Structure design

[loki3000]

hello,

can someone enlighten me on how to work in the strucure design workbench?
my final intent is to design a yacht cradle, used to hold the entire hull or deck of the yacht. similar to the one here:

http://www.yachtshippingcradles.com/images/cradle.jpg?145

but much more complex.

the profiles are more or less rectangular hollow with varying dimensions.
right now that's done with simple sketches and extrude (not me yet, the ones before me; mostly due to the lack of training) but i'm trying to learn the SD workbench hoping that it would somewhat automate/ quicken the process.

i've tried sketching a simple frame (box, but without using the grid option, as i don't see it applicable in the final design), but i've learned that i have to publish the geometry. the problem is that there is no such option nor in the part design where i made the initial wireframe nor in the SD workbench. i will consult online help though for it.

so, for starters, how time consuming is this publishing, when done on a larger level (maybe 100-200 elements)?
can you provide any best practices that i should follow?

i have a good basic knowledge of catia (part, asm, dft, much of that inherited from other cad packages though), but not advanced features (publications - solidworks doesn't have them either for example).
training is not (yet) an option and frankly i also doubt that the local VAR is familiarized with the workbench so much that they could do more then read from the training script)

 

[loki3000]

i've also looked at some videos at youtube, but they just use the grid option and specify the profiles.

 

[GELFS]

Hello Loki3000.
Generally speaking, any design consists of the following phases:
[ul]
[li]Conceptual Design[/li]
[li]Functional Design[/li]
[li]Funtional to Physical Design[/li]
[li]Detailed Design[/li]
[li]Drawings Production[/li]
[/ul]
CATIA follows this concept.

The method I use to do structure design is the "Skeleton to Model" method.
[ul]
[li]First, with the aid of GSD workbench, I create a Skeleton where each profile is represented by its centerline, each plate by a surface,... (Functional Design)[/li]
[li]Then I insert the skeleton in a CATProduct[/li]
[li]Next, I dress up the skeleton with structural elements (profiles, plates,...) with the aid of Structure Design workbench. (Funtional to Physical Design)[/li]
[li]Finally, I do all the detailed design (Endcuts,Cutouts, Coping, Drilling, Machining,...) (Detailed Design)[/li]
[/ul]
Note that, functional and physical model are associated ie if you change something in the functional model your physical model will be updated also.
That's how easy it is to use the Structure Design in conjunction with the Generative Shape Design to model a structure.

I hope it helps.

-GEL
Imposible is nothing.

 

[loki3000]

but do you need to publish actual spaceframe geometry? when in SD workbench, i got an error that said something about that (the geometry was just a square, drawn in part design though).
i vaguely remember a site on the internet that had a structure design tutorial, but i can't find it anymore.

thanks for the reply, you've been very helpful.

 

[GELFS]

Hello Loki300,
No, there is no need to publish the Skeleton.
What is the version you are using?
Note: To create a plate is better to have a surface support, made out of your square.
If you need any help is better to upload relevant docs(catpart and catproduct).

-GEL
Imposible is nothing.

 

[loki3000]

hmm, thanks.
it appears that i've misunderstood the whole thing.
i created a sketch in part design and transferred it into SD (insert part) and then tried to make a shape. that was the workflow i visualised with the real thing -- create multiple offset planes, sketch the required cross section and then connect those with lateral lines to connect individual cross sections. and then apply shapes etc. (this is more or less the solidworks way heh)

after creating the sketch i tried to insert shape, but i got error message: paste is forbidden, Impossible to create an external reference from unpublished element.

i will look into gsd, i don't know it currently.
version is r21 sp6

 

[jackk]

Loki,

You can get around the Publishing message by changing your settings:

TOOLS + OPTIONS + INFRASTRUCTURE + PART INFRASTRUCTURE: GENERAL page: turn off the 5th option to RESTRICT SELECTION TO PUBLISHED ELEMENTS.

 

[loki3000]

thanks.
is it difficult to create something like this on the pictures (note how the profile is curved in a secondary direction on the smaller picture -- that curvature is referenced by an outside hull shape and is paralell to it)
how would one go about making something like that (the profile in the pics is hollow squared and is currently only extruded/ swept, no structure workbench used. not my work though) with the structure workbench and its profiles?

 

[loki3000]

the files

 

[GELFS]

I cannot find any pictures in the rar file

-GEL
Imposible is nothing.

 

[loki3000]

works for me, there are pictures 1.jpg and 2.jpg

http://shrani.si/f/3a/T1/32ckN3zo/1.jpg

http://shrani.si/f/3o/C9/1FAf2okJ/2.jpg

 

[loki3000]

another source, if the above doesn't work

http://i.imgur.com/crg6ILV.jpg

http://i.imgur.com/IED6JLQ.jpg

in the first image the profile has to be paralell to an outside shape (hull).

 

[GELFS]

How would one go about making something like that with the structure workbench and its profiles?

What you need is to control the shape's profile orientation along the CL of it.

In Structure Design workbench and in the Shape command of it you must click in the [box]Reference[/box] field of it and select the Hull Surface. The shapes's profile axes will be perpendicular to Hull surface along the CL of it.

-GEL
Imposible is nothing.