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

Reply to
mtattar1
Loading thread data ...

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

Reply to
parel

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

Reply to
ken.maren

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.

Reply to
matt

Thanks! The VarFillet then loft procedure worked great!

MT

Reply to
mtattar1

PolyTech Forum website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.