Need help with loft error

Hello SW experts,
Im fairly new to SW and haven't had too many problems so far but this
one has got me stumped. I have tried to create the loft many
different ways and have tried with all the options like merge result
turned on and off.
I have reproduced a basic model and posted it here;
http://pichostonline.com/u/080729/a0b6b6c3b3.jpg to show what Im
trying to do.
Im trying to create a loft that goes from an oval section at one end
to a round section at the other end that terminates onto a curved
surface (cylindrical). My actual model is far more complicated than
this but this simple model was created using the same methods and
returns the same error that i'm experiencing.
The error is "Cannot make two planar end faces to cap the side sheet."
I have tried on both 2007 SP3.1 and 2008 SP4.? with the same error on
both systems.

Any thoughts on where im going wrong or how to get around this?
Thanks for the help.

 

Are you lofting surfaces or solids?

You could of course put a circle inside the cylinder, loft to that and
then let SW do the intersection.

TOP

 

Adam,

The problem you are experiencing has to do with the approximate nature
of projected curve - it is a curve projected on a surface lying on
that surface at a number of points but does not exactly bisect the
surface, when it comes to merging with the other solid, that tolerance/
intolerance gets in the way of the Boolean. Fortunately there is a
work around, and that is to work with implicit topology or edges of
the model.

Instead of projecting the curve onto the surface using the
Insert>Curve>Split and split the face with the sketch. Now try your
Insert>Boss>loft and it should work.

Second, you could Insert>Surface>Loft and do a Fill surface on the
edge of the end cap that is at the cylinder and then do a planar
surface face on the Loft start profile sketch, knit all three together
(using form solid command) then combine with cylinder.

I'm not quite sure about my explanation so I'm going to submit your
issue because this should work (from a user's standpoint)

 

The loft profiles need to have the same number of segments as a basic
rule. Break the ellipse into two segments and it will work.

ca

 

Thanks for the help everyone - TOP, I tried insert>curve>split but get
the same error as before, also tried the fill surface trick which did
actually work but presented problems further down the track when I
wanted to cut through the filled surface. In the end I settled for
your suggestion of putting the circle inside the circle and lofting to
that, which gave me a workable solution although not quite the exact
geometry I wanted. FYI, it is a race engine intake port and manifold
system that I'm playing with so the actual geometry of the finished
part will be fettled by hand anyway...

Clay - Im intrigued by your suggestion also as when I tried playing
with different start profiles, SW was sometimes happy to loft up to
the projected curve? No matter how many segments though, I still
couldn't get it to work with the start profile that I wanted to use.

Appreciate the Help!

 

You need segments on both ends, equal numbers, and how
you select (and where) each one probably matters. So does
their relative lengths as each segment will "map" to another
(getting each length just right can be interesting <g>).
Your resultant surface(s) (in this case as I grasp it from
your picture) would really be several developable/ruled
surfaces.
Some of the more fancy stuff allowed/required all sorts of
guide curves too but I don't think you need any for this
(even if SW uses/allows such).

Another method you might try would be to "project/translate/scale"
your circle past where you want the left-side surface to end,
generate the more simple surface between that circle location & your
starting curves (on right) and then trimming the result with
your pre-existing surface/solid.


http://www.ptc.com/appserver/wcms/datasheet/main.jsp?&im_dbkey=65285&icg_dbkey=841
We had an early release of CV's (Bezier) Advanced Surface Design (ASD)
long ago. Fun.

 

I want to reinforce TOP's advice. You should not define your loft
with a "potato chip" curve like you show. Define the final loft
section such that your loft penetrates the cylinder and naturally
produces the resulting intersection you need. Otherwise, you will end
up with a ratty surface prone to trouble.

If you need to control the loft-cylinder intersection closely, use the
projected curve to determine the location of guide curve to control
your loft and/or help define your final section.

 

Here's an example of using split to get the loft to flow..

http://www.zxys.com/misc/exhaustmanifold-zxys.zip

..

 

OK, Thanks again everyone. The least complex solution for what im
doing was to place my loft profile just inside the cylinder and let SW
look after the intersection.
ZXYS - I appreciate your time spent on that example - Its always
educational to look how someone else constructs various parts. In
your model theres a couple of features that I didnt even know existed
(composite curve & delete face).
Adam.

 

Kewl...

BTW, I added some more to it or made it into something else... so if
you want to see other methods,.. download it again... it's the -b
version

.. 8^)