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Hello,
sorry for asking this question in english, but my german is too bad to explain this in german.

I'm still new at inventor and I have a problem that I just cannot seem to fix, maybe someone here could help me..
I'm designing a catamaran, and today I modelled a hull (or a floater, not sure how to say in english), but its still a solid now and it should be hollow...so I tried the shell command but I keep getting the message 'edge has multiple or no solutions' (it says that with everythign i try; offset inside/outside/both, and allso with a very small thickness) I really need it to be hollow though because its handier for using the weight calculation...

So if anyone has any suggestions, it would sure help me a lot..
thanks very much  in advance,

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In my opinion, Inventor still has a lot of problems with shelling. Not all operations that should work normally, do that. Sometimes there's a reason for that, but many cases are like yours.

Sometimes dividing the whole thing to several segments can help, and then perhaps surface offsetting.

If you only need the weight of the hull, perhaps you can get there by working around with outer surface area, thickness and weight per cubic mm.

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hey,
..yea untill now I used the surface to calculate the weight, if it would be automatic it would be a bit nicer but well, I'll get over it 
thanks a lot for the reply

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Hi,

besides that, what Walter said is true:
These error results often out of fillets which would have an radius of less then zero in the offset surface. And maybe the error ocures on different parts of your solid, depending on the offset direction you chose.
If possible you may load up your file, and we can have a closer look at it.

By the way:
If you are looking for an english newsgroup, this link may help.

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Grüße Olaf

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I think, it's discussed there too, with a file upload.
It's a big world ..

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yea posted it on several forums, just to be sure.. i didnt quite expected that much reactions 
small world indeed

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Hi aswin,

i tried two things with your file:

- The scetch "boeglijn", end profile of your lofting, forms a microscopic small plane, IMO this is an obstacle for shelling. So my thouhgt was to remove it and change the loft. Loft is also possible "around the corner", e.g. from the deck (leftrail and rightrail together) to the front rib with "uprail" as rail. After deleting the sketch "boeglijn" i had to replace all the mentioned sketches by new ones and then succeeded with the loft, but sadly shelling didn't work either.

- Only after banning ALL splines from the whole part and changing ALL sketches to only straight and circular arc lines shelling worked.

I don't like the conclusion but it seems (also in other experiences i made) that splines and Inventor don't go together well. I would be glad to learn about the opposite. Is there anyone to teach me better?

Regards
Roland

[Diese Nachricht wurde von Doc Snyder am 22. Mrz. 2005 editiert.]

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Hey!
wow thanks so much for looking into my file Roland, you just cannot believe how much this helped me.
You are very right about that microscopic plane, I did this intentionally as a sloppy solution after an hour of unsuccessfully trying to loft the front part between the deck (left and right rail), the uprail and the end plane of the extrusion. No matter what combinations I tried, the damn thing just wouldnt loft! when I used the micro plane though, it did work.  (Being a perfectionist,I did not like this solution at all, nobody would see it was there, but I knew it was there...like a splinter in my brain  , but well..being my first model I tried to just forget it for now)

However, thanks to your previous message I decided to give it another try.. and after a few times It worked! I allso know now what I did wrong; its an incredibly dumm thing, but after selecting the final scetch 'uprail' I allways forgot to select the rail itself too, and now that annoying grey colored 'ok' button finally turned black!

But now I just got a final question; how did you change the splines into regular arcs/lines? is there a way to draw splines and convert them to something more usable for shell? Because I just find it soo hard to draw curved shapes using only lines and arcs.  for example the curves in my hull, the only way to get these things on paper as i want them too, is by using splines...they're so easy for making subtile curves...

anyways thanks a lot already, I'm relieved to know what I did wrong with the lofting..and even though I might not get a nice shell, I'm a happy lofting man now

regards

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Rumpf-einfach.zip

Hi aswin,

my sketches without splines were primitive, they consisted of only one arc from the projected longitudinal reference lines to the head tip. For ship design this is not sufficient.

In the meantime i have tried another hull model using splines for keel, deck and two ribs and - hooray! - it was possible to shell it. It seems to depend on very much details. I had to try several times and add the second rib sketch at the stern before it finally worked.

Best Regards
Roland

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