CATIA Frame

[HLai]

Hi,

I'm so-so new to CATIA in the sense that I've went through tutorials in a book but never applied the software into a project.

I need to draw a spaceframe in CATIA. When I was using Solidworks, I drew lines for where the steel tubing would go and then use the Weldments feature to apply a tubing of a certain size for each line. Is there a similar feature in CATIA?

Thank you very much,
Horace

 

[brengine]

Nope. You have to draw each 2D-profile and extrude. I found it easier to do a Weldment as an Assembly in Catia. It really isn't setup the same way as SolidWorks as far as handling Multi-Bodies. Catia handles Multi-Bodies superbly, but DDS had a different focus for the usage of Multi-bodies...and Weldments wasn't one of them.

Also, Catia Part files have no CutList generation capability. You can create a Bill of Material (and use that as a basis for the Cutlist) if done as an Assembly (although it'd probably be easier to manually type in the Cutlist values to a table in Catia).

As usual with Catia, I've read that there is a separate Add-On license for Weldments, but I've never used it.

 

[Azrael]

As mentioned there area a lot of workbenches so it would help to know what you have.

Don't understand how it works in SW, do you mean that you define the tubing dimension in a weldment feature? By the way welcome to the Catia world Keep in mind that Catia is process oriented and not feature oriented and everything will be fine... almost

This is how I would do it, I would create the space frame with "Structure Design" workbench (dedicated for beam creation) and then go to the "Weld Design" workbench to define the welds.

But depending what licenses you have there are other ways to do it, you can do it with the standard "Part Designer" and define the welds in 3d or drawing but what you will miss from the "Weld Design" workbench is the automatic edge trimming depending on weld type and adding the weld material as a solid feature. The "Structure Design" workbench is just a fancy beam create and trim set.

 

[HLai]

Azrael - "do you mean that you define the tubing dimension in a weldment feature?"

Yes, that's exactly it

I can't find any good tutorials on the Structure Design workbench. I have both the Structure Design and Weld Design workbench.

Right now I have a wireframe model that was made using the "Wireframe and Surface Design" Workbench. I was able to import that into the Structure Design workbench. I am now stuck and have no idea how to make my lines into tubings.

Do you know of any good tutorials online?

 

[Albigger]

The CATIA help files (if installed) are usually pretty explanatory, often including some examples.

I can't speak for the Structure and Weld Design workbenches (I haven't used them) but you might want to start there.

 

[brengine]

In SolidWorks you can draw a sketch on a 2D plane *or* 3-dimensional space.

For Weldments, you Insert a new Weldment Feature and simply follow the dialog...select the Sketch Line(s), select the 2D-profile that should be "swept" along the Sketch Line(s), and Select a corner treatment (i.e. how the ends of the structural members are to be trimmed to adjacent members).

It has other automated tools to insert caps at the end of tubing and/or Gussets (without needing any sketch at all).

How the Cutlist works...Each member is a separate body (in the part file). You can assign properties to these members (Description, Material, etc...). Then in the 2D-Drawing, just select Insert/Cutlist Table, and you get a linked table (that includes item number, cut length, and quantity if desired).

 

[Azrael]

-Create a Catproduct and insert your wireframe space frame
-Go to Structure Design
-Use the Shape feature
-Set type to support and pick a line or multi select the wireframe by holding ctrl
-In the Material tab choose wanted section.. say a Pipe
-ok
-If needed cut/merge parts (merge, cutback, cutout)

For this case I would not use the weld design workbench instead go direct to Assembly Designer and create weld notes or on the drawing

 

[HLai]

Hi Azrael,

Thanks for the tip, it helped a lot.

Would you know how I could create custom pipe sections?

Thanks again,
Horace

 

[Azrael]

Check the documentation, it's table driven with catalogs. Think there is a section in the documentation about sections that is important due to correct element naming i crucial and there is a section about catalogs to set it up correctly. That's the right way to go but you can always go to the component library and change existing setup to fit your dimensions.

 

[HLai]

I finally got around to installing the online help files. I look over it and was able to create catalogs. I was also able to create a tubing profile using sketcher. But I can't apply any of this to the shape tool in the structural workbench. I have no idea where the catalog for the shape tool's profiles are, nor do I have a single idea of where to begin to search.

 

[HLai]

Hello,

I'm still having zero luck with getting custom profiles to work for my v5R19. I see that there are no more replies and am just hoping there might be some tips after this bump.

Regards,
Horace Lai

 

[Azrael]

Check in your install path: ?:\Program Files\Dassault Systemes\B19\intel_a\startup\EquipmentAndSystems\Structure\StructuralCatalogs
There you will find what you are looking for, I would suggest that you go to the AISC folder there is DesignTablea folder, note the AISC_Pipes.txt, try to edit it. Not sure if you need to update anything, give it a try.

 

[HLai]

I've tried that before and I've tried editing the catalog on that AISC folder as well as the catalog in the StructuralCatalogs folder. Didn't work.

I did notice that the profile sketches in the ModelsResolved folder match up with the profiles listed in the Shape tool menu, where as the design table for Pipes have more values in them than there is listed in the shape tool menu. So I've just tried editing the dimensions in one of the section profiles in that folder and still no luck. Adding more entries also yield no luck either, either to the AISC catalog or to the ModelsResolved folder or both.

 

[Azrael]

I'm not sitting with that license right now but if I recollect you should add your entry and run a script to resolve the parts, think that is described in the docs. When I get the possibility I will try it again to fresh up my memory

 

[ferdo]

Hi,

If you would like to use just part design and assembly design workbenches, you can use this

http://www.megaupload.com/?d=51EXLKQQ

(I suppose you know something about assembly design so you can handle part in an assembly).

Regards
Fernando

 

[HLai]

Hi Fernando,

I don't think that's relevant with the structural design profile issue I'm having. Thanks for your time anyways.

About the issue: I found where it says I have to resolve the parts, but I don't know how to do it.

online/CATIAfr_C2/sr1ugCATIAfrs.htm

In the help files there it says I have to do a bunch of stuff in the command prompt and know the CATIA environment file name.

Does anyone know what the "environment file" is?

This is getting more complicated than I thought, and I haven't even gotten to the point where I put the model in beam elements and analyze it in CATIA. I'm seriously thinking about going back to Solidworks to do my iterations and analysis and then putting it all in Catia in the end.

Horace

Regards,
Horace Lai
Chalmers University of Technology

 

[Azrael]

Go to start->catia->tools->enviroment editor... there you will find the enviroment file. It's just a txt file with various settings, you can open it with a standard text editor also.

Judging by your signature I guess that you are from Gothenburg, why not contact your local Dassault office? or wait until I get a chance to try it again

 

[CBunes]

The environment file is like a library file that you use to launch catia with. If you inspect your shortcut to start Catia you will notice that it references something like this:
-env some_name_here -direnv "C:\Documents and Settings\All Users\Application Data\DassaultSystemes\CATEnv"

some_name_here is the name of a .txt file that you'll find in that directory. It contains all paths to your Catia installation, where your settings files are located and paths to any additional plugins you've installed.

Without this environment file Catia wouldn't really know where to find anything it needs to function.

Hope this clears up things a little for you. Oh, and do what Azrael says: Contact your supplier. They should be able to help you out with documentation and guides.

-----------------------
Christian Bunes

http://www.plastal.com/

 

[HLai]

Nope, can't get it to work. It keeps saying it couldn't find the directory for my Part file.

I have called the local Dassault Systemes office in Gothenburg but they were not able to give me the answers. Only told me to check out the help files and the companion. I'll have to see if I can get access to the Catia companion.

Regards,
Horace Lai
Chalmers University of Technology