chamfer or swept cut on an elliptical edge ?

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

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

Dave

Rocco wrote:

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 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

Rocco wrote:

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.