More concept section problems - change of approach needed?

[trimboy]

Still struggling with v5 and have come to the conclusion that creating a section layout is very time consuming, if not nearly impossible. Have spoken to lots of people here "in the know" and they all have suggested that you don't need to create sections for anything! Just create the model in 3D and then if there are problems, it can be modified.

My question has been to all of these people - how do you know how a complex part such as a door trim is constructed without sections? They all have said that a 3D model is better than a section model for packaging. Now this goes against everything I know about engineering - even the most basic model is started with a section.

Went to see a guy yesterday and he showed me a fantastic model he has made, all linked with parameters so you can change one bit and all the rest of the assy follows - however, when asked how he set it up in the first place, he showed me a section on a piece of paper that he had used!(he got this from someone else).

Is there some kind of conspiracy going on here, as everyone I have asked seems to have made models once the basic design has been sorted out - no one has actually produced the section themselves from which they have been working! Apparently, as this guy said yesterday "you know what the section is going to be so you don't have to produce it" - what if you don't know what it will be? These people are all saying the same, like they've had their brains taken out!

This is proving very tiresome, as we have an A surface and need to do feasibility sections for technical input to design - we can't model parts in 3D with a surface that may not be in the right place, only to find that the surface is wrong and has to change once we have done the 3D models! By then the A surface will be frozen and can not be changed.

I have started to doubt my own engineering experience here as I can not visualize how parts go together just by looking at a surface and then starting a 3D model. It feels like I am surrounded by guys here who have no real engineering experience, and they all have the same mindset. Talking to some guys on the body group, they say they never use sections, even in V4, but their parts seem to be simpler - I can't believe this!!!

Advice, anyone.........?
Thanks,

 

[abeschneider]

If I understand your problem, then I use sections all the time as the basis for my modeling. It's indispensable, as I'm the original creator of our models (I am not, say, editing a part that fits into a machine someone else has already designed...)

A very basic description of what I do is I create a "skeleton" Part, composed of a number of sketches, datums, and full of the "knowledge" or logic that drives the model (say, a complex machine).

Since many of the major subcomponents or subassemblies directly relate to the skeleton, the skeleton is often the topmost component of my assemblies and subassemblies. I use Contextual Links to bring in the appropriate geometry into any specific part.

You can read more about this approach if you search for "skeleton" here or especially on another forum:

http://www.catiav5forum.de

 

[flangewiper]

I use sections in my designs too - I'm doing automotive exterior trim parts. If I'm working up a few quick sections to use as a guide to start off a design, I've found that turning the 'Create Datum' button off helps and then just create your lines in 3D space using a support plane in GSD seems to work well.

Ok so you've got no history to your section but at least you can delete or trim back individual elements without it all falling over and you don't really need history if your section is only used as a design guide. You can cut sections throught adjacent geometry with the datum off as well if they're not likely to change. This method has vastly increased the speed I can create a section without having it keep falling over.

I did try using sketches to create the sections but just got in one a hell of a mess so for me the above method has worked very well. It would be better if you could just work on a 2D plane like on V4 so you didn't have to keep specifying a support plane and before anyone says it, I know you can use 'Work on Support' but again I found this messy. Just create youself individual Geometric Sets - call them Y150, x2400 or whatever, define your support plane, turn the datum off for all subsequent commands by double clicking it, and away you go. Remember though to turn the datum back on when you create your 3D geometry or you end up with a load of dumb elements.

If you then need a section that updates as you go along, create intersects in another Geometric Set with the Datum turned on and keep you old section just as a look/see guide.

 

[trimboy]

Excellent - thanks for the info - I was beginning to think that the idea of sections was dead!

 

[flangewiper]

Section Engineering dead? Never! I've made a 20 year career out of it!!!

 

[solid7]

No sections = costly errors. Part of a corrupted culture of faster and cheaper. Everyone these days seems to be a "tube jockey".

I'm not sure that I understand how anyone can claim to be creating accurate data without sections, but if you get some more info on that, by all means, post it.

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

 

[trimboy]

I agree totally! No sections = no idea! I've just gone onto the v5 having spent the last 15 years on v4 (and previously v3). I'm on the job being coached by guys who have come straight from college and have done the v5 course. They've spent some time getting hot on the 3D stuff, but of course they are not engineers and just stare at you blankly when you ask how they propose you should design a complex part without sections. It would have been better also to have guys who have experience in real world engineering, perhaps on v4, so they could answer questions like "on v4 I did it like this, how do I do it on v5?" This is the future........!

 

[solid7]

I not only still create with sections - but I go one step farther, and use the wonderful thing called "geometrical set" to organize all my data, contextually. I love being able to drawer reference data, and pull it up at any time. And what's more - V5 allows you to reference the geometry even better than V4. Not as easy to find via power input as in V4, but better for organizing overall. (love the "folder" and "subfolder" approach)

By the way - it is not time consuming, nor impossible to create from sections in V5. One of the easiest ways that I have found, is to extract geometry from the assembly, straight into the detail part. It will come in as dumb solids, each part in a separate PartBody. You can then extract and delete as desired.

I submitted a tip sometime back that you might find useful for importing data to be used for sectioning:

http://www.eng-tips.com/viewthread.cfm?qid=142427&page=1

I'm not sure if this is supposed to work like this, or if it's a beneficial "bug". (couldn't find it in the documentation, and I found it by accident) Either way, it's great and I use it alot. Just remember that the example given used surfaces, and to get a solid in your detail model, you need to select the PartBody - not an individual face.

Good luck, and I hope that helps.

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

 

[trimboy]

OK, thanks for the advice! I'm trying the flangewiper method at the moment - using intersect with the create datum switched off so I create dead geometry. I am cutting through some carry over V4 bits which seem to take an eternity to cut through (I've managed to read most of the BBC news website in the time it takes to just cut the section!) Once I have the dead intersects I will then project some of this into a sketch to create fixtures/fittings etc which are then parameterized. The guy sitting next to me has managed to to a small section like this and it only took him 2 days!!! I'm not kidding, there must be something we are doing wrong here and we're running out of time as management are talking about doing the feasibility in V4 now!

 

[Azrael]

Hi Trimboy

Have done some testing in this area and there are some problems working with section in V5.

The intersect method works fine if you have a limited amount of parts. Tried that with hundreds of parts for master sections and it crashes, due to it caches/copies all bodies into your body, even with datums turned on it will copy the parts and when the intersect is done it will delete them but it drives the memory through the roof.

So I tried using sectioning, with DMU space analysis there is an option to export the section as a part, this will give dead curve, whiich is ok for this. But the section is based on the representation, meaning not exact, but if the tolerance is set highest possible, the system will recognise curve types on drafting (that a circle is a circle and so on). But this curves can´t be used a construction elements.

So my recommendation was to use the sectioning approach to secure the areas and use the intersect approach to deliver usable sections for engineering. These two different section has to be separated into two different sets, the DMU section set I set to no pick so it was clear to not use it.


Are there other suggestion on how to handle large assemblies? The limitation we have is that catia don't have a tool to section large assemblies exactly.