chamfer or swept cut on an elliptical edge ?

I have something that should be easy to do, but is not in practice. I
have a tube cut at an angle. I want to bevel the angled edge (now an
ellipse) all the way around for weld prep. The chamfer function balks
at this. A swept cut would seem to be the way to go, but I get all
kinds of funky cutting geometry. Any ideas? I can email a part if you
want a look-see.
I'm using SW2006.

 

Yep...didn't work.

What does work though is to place a new plane, parallel to your beveled
surface, and offset by the length of your chamfer. Then use that plane
to create a split line on the cylindrical surface. You can then do a
45deg draft on the resulting surface.

Let me know if you want me to send the model I just created.

Dave

 

Rocco wrote:
Any ideas?

Since it's only a chamfer for a weld, could you just do it as a
"Distance-Distance?" I know it doesn't make a consistent width chamfer
all the way around, but how much trouble do you want to go to....

Steve R.

 

Excellent, hadn't thought of that...BUT what plane are you using for
the neutral plane when you insert draft? If I use the angled plane I
get correct draft at one end of the ellips and opposite draft at the
other end.

 

"Since it's only a chamfer for a weld, could you just do it as a
"Distance-Distance?"

Nope, chamfer refuses to do it.

 

I used the new plane (the one also used to create the split line)

 

I tried it before I posted to your message, and "Distance-Distance
worked fine. Maybe what I tried is not what you're trying to do.

Steve R.

 

OK here is the behind the scenes update: many thanks to Dave, his
method works like a charm on a round end, but the angle cut end won't
play ball.
Any other ideas?

 

I tried it also and chamfer "angle distance" do not work, but chamfer
"distance distance" do work (2006sp4.0).
\/\/im

"Rocco":

 

Correction: it only works for me when both distances are the same!!

"Wim":

 

okay, a lofted cut with 4 profile sketches (1 at each quadrant) with
elliptical guide curves seems to work, but there must be an easier way!

 

Here is my way

-On the face of the cut sketch an offset the dist of the chamfer.
-Offset a plane the distance of the chamfer and create a sketch using
the 'intersection curve' of the outside of the tube
-Loft a surface between the sketches
-'Insert-Cut-With surface' and flip the cut to cut the desired section

I tried to do a lofted cut but it does not seem to have a flip cut
direction option...Bummer Dude! Although you could use lofted cut 'thin
feature' and make a really thin cut if you don't have to be dead
accurate and then remove the excess body, it takes a couple of steps away.

Ben

 

That worked! Simpler than four profiles, but still had to add an
additional sketch to make a guide, as a simple surface loft and cut had
a slight concavity to it without the guide....probably would not matter
if simply making a weld chamfer.