Parametric Design 2

So what you're really saying, is that you're a former Pro/E user, and you want to do things like a Pro/E user? (you're not a former or current John Deere employee, are you?)

I may be lost, but are you saying that parametric design and skeletons are synonymous?

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CAD design engineering services - Catia V4, Catia V5, and CAD Translation. Catia V5 resources - CATBlog.

Yes, Im a ProE user but never been a John Deere employee.
I'm really tired of all Catia people thinking that ProE users always want to do things like thay done it in ProE. I'm very open minded and tries to use every benefits and strenghts of every CAD program that I use. I do belive every system is uniqe and there is not one system that is the best in all areas. In some cases maybe SolidWorks is the best (easy and fast to use and learn), ProE is really great in creating pattern and I like the flexibility that Catia provides.

Yes, I say that I drive my skeletons with parameters. In most of the cases I don't use external references. Instead I create relations between parameters at different levels in the product structure. External references are great in some cases but I large structures (more than 5 levels in the structure and thousands of parts) I think Catia have problem updating external references (have to use synchronize). Relation driven structures are in my opinion more stable. In some cases I let a design table control all parameters at top levels.

How do you define parametric design?

Akesson,

Everytime I attend a COE meeting, it seems that more and more companies are using the 'sketeton methodology' you described (or at least some form of it).

Based on my experience, I strongly recommend it for any company with several engineers/designers working on same the product.

I agree, the skeleton method work good in V5

But I would also like to adress part modeling techiques.
I tried the GM chunky modeling for thin walled designs in V5 and must say that it works even better in V5. Does anybody have other experience? I tried to get a modeling recommendation from our Dassault contact but I get the feeling that they don't have a clue what I'm talking about.

Akesson said:

I'm really tired of all Catia people thinking that ProE users always want to do things like thay done it in ProE.

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Whoa, there, fella. No need to get bent out of shape. I was simply pointing out that I've heard this all before - almost always from Pro/E users.

Akesson said:

Yes, I say that I drive my skeletons with parameters

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No, that's not what I asked. You seemed to be inferring that skeleton design was "true" parametric design. (to which I would have taken issue) In fact, parametric design does NOT depend on skeleton methodology. This is just one way to utilize parametrics.

I don't believe in blanket statements, such as "this method" or "that method" should be used and preferred to all others. The reason why skeleton methodology isn't used in Catia more, is because the major business partners (who pay for the development of Catia) do not, by and large, employ this methodology. This is reflected in the majority of Dassault training material, and the "best practice" advice that is handed down. Since particular groups get first say in the bulk of the development decisions, expect the methodology to be "flavored." (as is reasonable)

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CAD design engineering services - Catia V4, Catia V5, and CAD Translation. Catia V5 resources - CATBlog.

Hi Solid7,

Thanks for all input in this thread.

I'm still not sure how you define parametric design and if you do not even use a skeleton part to at least position parts (with plane to plane constraints). How do you then keep you lagre structre stable (no constraints between to parts in a product)?

And I havn't said that there is one method that could be used in all cases and by all users. What I did say is that there are some advantages (in my opinion) with skeleton methodology.

Maybe you could describe the disadvantages with skeleton methodology in more detail than just the fact that the major business partners not employ it?

Akesson said:

I'm still not sure how you define parametric design

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It doesn't really matter how I define it - it's already a term in use, coined by someone else. The best that I can do, is scab a definition from one of the many companies who are using "parametric" modellers. At any rate, my main point is, "skeleton" design, is not, in and of itself, the de facto definition of "parametric". It is simply a way to utilize parametrics. (because the system is already parametric whether or not you use skeleton methodology)

Akesson said:

if you do not even use a skeleton part to at least position parts (with plane to plane constraints). How do you then keep you lagre structre stable (no constraints between to parts in a product)?

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Stable compared to what? In V5 assemblies, "stable" is a foreign word. (getting better, though)

Why would you want to force someone's hand to NOT use constraints? You mentioned the use of planes - logically, we can argue that every piece of support geometry, including sketches, can be considered a "skeleton", but that's not what we're really talking about. (at least not) My assumption is that you are talking about skeletons controlling major aspects of the design, either in context, or via use of constraints, whereby the "skeleton" data is held in an external file. (not a major 3D solid component)

Akesson said:

Maybe you could describe the disadvantages with skeleton methodology in more detail than just the fact that the major business partners not employ it?

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Sure. Skeleton methodology isn't such a bad idea. It works great in small departments where everyone is pretty much in-touch, and has a clue what's going one. But, that being said, put it in place in a large corporation, where people within the same group may not even know everyone else's name. Here's what I see as the major problems:

1) Potential loss of "in-work" data. (how annoying is it when you're first working with an assembly, and you haven't quite mastered the "save as" function - only now you're messing with other peoples' work, also)

2) Uncommunicated changes. You come to work, and your file isn't the same as it was yesterday. (see above)

3) Broken link nightmares. (no explanation necessary)

4) Higher learning curve in mastering configuration control concepts.


I feel that the confusion created by using the "top down" design method, alone, is sufficient reason to insist on all due dilligence before accepting it. While the advantages seem obious at first, this is a very complicated and involved process. You are now talking about a design methodology where one change can completely destroy the design intent and integrity of an assembly, whereas the bottom up method will, in most cases, only diminish the assembly. (yet it has its own problems)

I've seen this method used, usually with much confusion. On paper, great. But in the real world, it becoms a chess game, and often ends up costing the money that it was supposed to save. My exposure to "top-down" design, showed me that even after several years, many users still didn't have a grasp on the concept, which resulted in lost time - either fixing their "changes", or giving it to someone else who DID understand.

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CAD design engineering services - Catia V4, Catia V5, and CAD Translation. Catia V5 resources - CATBlog.

One thing is for sure, you and I don't talk about the same methodology!

With "my" methodology each user work bottom up and then later all parts are "connected" to the assembly. You're talking about a methodology using external references and parameters that could be used (in my opinion) far down in the structure but not as an overall skeleton.

I've worked with companies that builds trains and other large structures and many users using similar methodologies. Maybe there is different maturity to new modeling techniques on different sites/companies?

"1) Potential loss of "in-work" data."

I don't see how skeleton methodology makes the save procedure worse....

"2) Uncommunicated changes. You come to work, and your file isn't the same as it was yesterday. (see above)"

True, the skeleton is mastered by one person that propagetes changes. Which I see as a strengh.

"3) Broken link nightmares. (no explanation necessary)"

I said earlier that I don't use external links (copy paste) but instead relations between parameters at different levels in the product structure and therefor you don't end up with any broken links!

"4) Higher learning curve in mastering configuration control concepts."

True! I can agree to some point that it takes time for some users to understand the methodology.

I'm not sure how you can use the "skeleton" method "using relations between parameters at different levels" and not have links. Anytime you associate something in one CATDocument to something in another CATDocument, you are going to create links. That is just the way that CATIA works.

That being said, we are currently using some of this "top down" approach in a relatively large scale. Change Control, and a VPDM system are essential tools when working this on a larger scale. We currently use VPM for this.

Yes,it is a higher learning curve, but we started our V5 experience without links, just so the user's could get past the initial "V5 Learning", then we started using the advanced functionality. And we don't use linked parts for everything, just for the critical structures.

I'll second catiajim on his comment. Curious as to how anyone could utilize the "skeleton" method and not have links. They're just different Kinds of links (ie: CCP, KWE, Instance, Constraint, and ViewLink...)

COE has a good series explaining links in Catia, by the way. One of the series can be found at:
The series continues in other months' archives.

Hi,
in our company we use "skeleton" , which is called reference model here....
It worked in Catia V4 with no links, now used in CV5 with links via PUBLICATION...I’m surprised there is not any mention about it in this discussion...
It works well; one disadvantage is that there isn't possibility for sorting PUBLICATION in the tree.

I must say, that as we work on airplane in many groups on many assemblies, I can't imagine work without skeleton...in our branch its necessity...

Not every part is made with link to skeleton, but I model it in absolute position and in assembly could constrain, but on every par I use FIX. We have quite bad experiences with constrains (makes work slow, tearing...) so if possible we constrain part on its position, then delete constrains and make FIX...

Good luck fellows

Hi All,

Sure I create links between documents but I don't use external links created with copy/paste special. Instead i create relations between parameters with the formula editor.

I have all main parameters at product level.

Some of these parameters I also have in the reference part (skeleton). I use these parameters to positioning planes, creating other kind of support geometry etc. In some of the sketches I create ref dimensions that I link to parameters (use Catia as a calculator).

Then I create relations between the parameters of the product and the parameters of the skeleton part. Active in the product.

Then I create the parts with wanted parameters. Making sure that the part obtain the flexibility that I would like it to have.

I assemble the part in the product.

Last but not least I create the relations between the product and the part. Active in the product.


By doing like this I can add the "intelligence" to a part at a very late state of the project. Another benefit is that you don't end up having to do "synchronize" and having broken links.


I feel that this is difficult to explain just in text, the best thing is live demo...

I agree with catiajim that it important to have well defined change controls etc. I've used this metodology both with VPM and Smarteam (both having their limitaions...) with products containing +10k parts.

heidy, using publications is great. I publish all planes I use for positioning and other parameters and geometry that I use as refernces and later may replace.

heidy - you can sort the publications. it is a bit cumbersome, but for skeleton parts it is worth the time. In the publication menu you can export to file the publication list. Edit this list in notepad. Delete all the publications in Catia. Import the sorted list via the publication import button. Reconnect the items.

Regards,
Derek