sheetmetal, elipse

Hello,

I have an eliptical shape and would like to turn it into a sheetmetal
feature. When inserting the sheetmetal feature there are bends found and
there is consequently no flat layout.

Is it possible to use elipses into a sketch of a sheetmetal part? I
looked into the help file. There was nothing indicating it is or it
isn't passible. Maybe someone can give me an answer.

I'm using 2004sp4.0

Johnny

 

Just like with a cylindrical sheetmetal part you have to have an open
elipse. It only needs to be opened by .001 or less but open none the less.
Then have an offset sketch of the same elipse (Probably convert entities to
a parallel plane) then use lofted bend between the sketches. You will now
have a flattenable elipse. Mind you I don't know exactly how accurate the
flat pattern is going to be since an elipse is an approximation anyways,
time will tell.

Corey

 

Hi Johnny,

I read in a german forum that the SWX-sheetmetalfeature has problems
with elipses and splines.
I use tangent radiens to create this kind of sheetmetal.
Maybe you understand german you can read following artikle
http://ww3.cad.de/foren/ubb/Forum2/HTML/003275.shtml
otherwise my sample helps
http://www.construction-3d.de/misc/ellipse.gif
http://www.construction-3d.de/misc/ellipse.zip

--
best regards


Steffen Tschirch


Hildesheimer Str. 401
30880 Laatzen

Tel.: +49 5102 909634
Fax : +49 5102 914732

http://www.cad-zeichen-buero.com

 

Steffen could you summarize the article in English for us.
Corey

 

the importent message of this article is that you can't flatten ellipses
in solidworks at themoment. There is a sample
http://ww3.cad.de/foren/ubb/uploads/Oberparleiter/testblech.zip
but the ellipse isn't flattened.

 

Try the method I described above it is possible I just did one. Maybe I
should make one exactly like theirs.

Corey

 

Correy,

Your methode is the most succesfull. I had some glitches to conquere
when converting the part to this part. Now it works.

Do you know how accurate het flat layout is?

Johnny

 

Unfortunately I don't know. I think it will depend on the actual tooling you
use to create it, it may be accurate but it will also vary depending on your
bend Allowance. Trial and error will tell, but when you find out let us
know. Just don't send it out to the shop expecting it to come out perfect.
If you don't expect too much you won't be disappointed.(This view should not
be applied to everything mostly aproximated shapes in SW). Did you know you
can make flattenable helixes this way too though for a flat pattern you will
need to only have one revolution

Corey

 

If you put an ellipse (partial) in a Base Flange Sketch you will get
and unsuitable geometry warning and not a feature.

 

I don't get it are you two trying to find another way to do this? Was the
working solution I posted not adequate or something? (you don't use a base
flange at all.)

Confused
Corey