sweeping surfaces vs sweeping boss/base

It's so stinking frustrating... I'm trying to sweep a surface (open)
around a 3D sketch. It will sweep a pretty complicated solid around
with no apparent problems but when I go to do a simple surface (even a
straight line) it won't sweep. It will sweep a closed simple surface
though (triangle, cirle, etc) but *won't* sweep my original complex
solid (which swept fine as a boss). What gives? Am I missing
something fundamental here or is it just a quirk in the 3D spline I'm
trying to drive around?

Joa

 

(Joa) wrote in @posting.google.com:

I know it's a cop out answer, but the more complex something is, the less
likely it is that someone can help you from a word description. All we can
do really is offer general suggestions.

With sweeps, SW makes a series of planes which have some relation to the
path and guide curves if present, then it re-solves your profile sketch on
each of the planes and makes a loft from the intermediate sections. This
means that your sketch relationships can cause a sweep to behave in ways
you don't expect sometimes. Also in 2004 they have removed some of the
pierce point requirements which means that some sweeps that used to fail
for lack of a pierce will either fail because of screwy geometry or maybe
work. Still, I recommend that you use pierce relations to make sure your
sketch is tied to the path and GC.

People have written a lot of stuff on this, and I can't do it justice in a
short post. Maybe the best way for you to get meaningful help is to post
your model on a web or ftp site.

good luck

matt

 

You lost me when you said it would sweep a pretty complicated solid around,
but then a few sentences later said it '*won't* sweep my original complex
solid (which swept fine as a boss)'. Did you mean it *wont* sweep a surface
using the same section as the original complex solid?

Anyway, there are a couple of things that might be happening:
1)bugs. This is common in 2004 - if at first it doesn't execute as a
surface, try it as a solid (someitmes even closeing the sketch and try it as
a solid). I have samples that I've reported. The workaround is simple -
sweep as a solid (don't merge with other bodies), then 'delete face' the
ends and extra sheets to turn it back into the surface you originally
wanted. This is, of course, odd because in previous releases we had better
luck sweeping as a surface when the solid didnt work.
2) Loft issues. If your PATH has any sections that are splines (or were
made from projected curves, which could very well become splines even if the
consturction curves are analytic), that section in the final sweep will be
lofted behind the scenes. This brings in all sorts of extra stuff relating
to curvature of the path and isssues with the centerline loft command (which
is invoked behind the scenes). Oh, you said the path is a spline... well,
that is too much stuff to go into right now (I've only got a minute)
3) I presume this is not a sweep with guide curves. If it is, there is a
whole world of new stuff that might contribute.
4) Initial angle of the section plane to the path can cause problems, though
I don't expect that you have these issues because it works as a solid and
not as a surface.

Seeing the file helps, though my guess (without seeing anything) is a bug
becuase I've witnessed that firsthand. Its either that, or check
thecurvature of the path and see if there are any freaky bits.

Good luck
Ed

 

(Joa) wrote in message

have you tried using "path alignment" ?

 

THanks for all your responses. Let me play with the model a bit more
to see if I can clarify a little better....

Joa