Catia V5 Newbie 1

[thixoguy]

Hi All,

I will be starting a new job where I will receive some V5 training in the near future(I come from a UG background).My question is if I import a part file(iges)how do I sew or stitch it into a solid? I have tried to use the sew feature but that seems to sew a surface onto an existing solid,my file consists of individual surfaces.

Thanks in advance for any help

p.s. this is an extremely informative site.

 

[nadam35]

good question,

i have often wondered that myself...

 

[solid7]

This is not "sewing" as it is in UG. As you have said, sewing in Catia is used to joing a surface directly to a solid body. You would need to use the "join" command under the GSD workbench. Before doing that, however, you need to run a surface connection check, and see what your minimum join tolerance is, and decide if that is acceptable for your purposes.

Once you get a join, you should check for connectivity further, by trying to extract boundaries on the join. If any boundaries appear, you have problems.

Start off by looking up the join and surface connectivity checker in the help menu. If you have any questions, post a follow-up to the forum.

Hope that helps.




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[thixoguy]

Thanks for your input solid7,I will look into what you have suggested.

 

[thixoguy]

Solid7,

I used "join" in GSD and checked connectivity by trying to extract edges; no edges, so I assume I have a solid.

My next question is twofold
1. In the history tree I still see OPEN_BODY.1, does this mean I still do not have a solid body?
2. When I go into part design workbench and try to add a fillet to my joined surfaces,the options available under dress-up features are greyed out, leading me to believe I still don't really have a solid body.

Again, thank you for your "Solid" input (pun fully intended)

 

[solid7]

A join is only a volume. You must use it to form a solid body, by using the "close surface" function in Part Design.

You can't do anything in Part Design without a solid body.




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[thixoguy]

Solid7,

Thanks for your help... worked perfectly

 

[Jaso]

Does anybody has a good method of transfer from catia 5 back to catia 4 . I have a iges only. I can't change any settings in C4 and I have to manualy rework many faces because of gaps. Thanks Solid7 for your help.
Jaso

 

[solid7]

There is a mismatch in the tolerance of the modeling kernel, between V4 and V5. It is about 95% likely, on any given (complex surface) file, that you're probably going to get some gaps that need manual repair.

I wish that I could give you better news, but that's straight fact.

And to answer your question - just save the file as .model from V5. (you do have that feature, right?)

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[TurbulentFluid]

thixoguy,

for your original question use "Heal" or "join" from WF&S and then "Close Surface" from Part Design, that should do the trick. "Heal" will try and sort out the little gaps that come from IGES conversion... sadly, if they stay, then sink into manual repair... :-(

Tho there's a trick that sometimes works. You can increase the gap tolerance only so much and after that it won't create a solid. The trick is to scale your surfaces so the gaps between them are still smaller than tolerance, then make a solid, then scale to the original size. Sometimes this works very well!

Though, as I often use Catia and I-DEAS on the same model I found STEP format to be much more rewarding than IGES as it's understood as manifold solid by Catia and solid by I-DEAS. Hope this helps!

PS.
The existance of "open Body" in Catia doesn't mean you don't have a solid. Without enabling hybrid design, Open Body in the Tree is where all the surfaces are stored, regardless of whether they have later been used to make a solid.
PPS.
The Tree isn't always the History Tree. It CAN be, but unless you enable it as such, it's not. It's very different than UG logic.