fancy chamfer

Hi,

I'm trying to create a variable-sized chamfer around a horseshoe-shaped
part. The chamfer size is a function of where along the edge you are.
I've tried a few things but nothing simple. The to-be-chamfered edge
currently consists of several distinct edges. Lofts and sweeps seems
to be the answer but can't get anything to work.

Any ideas from the experts?

Thanks in advance
MT

 

Option1:
Create a cutting surface knit from smaller surfaces and sweeps that are
created with construction planes created at the ends of those distinct
edges
Insert>Surface>Loft/Sweep/etc
Insert>Cut>with surface
Option2:
Variable Radius Fillet the edge. Create a surface loft between the
edges of the fillet and then Insert>Face>Replace Face

 

The other thing that has worked for me in the past is to use to split
lines where you want the edges of your chamfer and delete the face in
between. Then use the fill surface to create the chamfer. If you want
that chamfered surface to be flat, simply choose contact as your edge
option. If you would like the chamfered face to have some dome to it
you can easily add contol sketches to select in the fill surface
command. Send me the part if you would like me to take a run at it.
Include a image of exactly what you want.

KM

 

The easiest thing to do is to use a variable radius fillet to create the
edges of the chamfer, then use Delete Face to get rid of the face of the
fillet, then create composite curves on the two edges and loft between
them, then trim the ends. It works like the split lines, but takes less
time.

 

Thanks! The VarFillet then loft procedure worked great!

MT