Problem with chamfer round object
Hi! I suspect you may need to select the three connecting edges together to create one chamfer. Another approach is to use a brutal technique of Offset, Split, Delete Face, Loft, and Stitch.
- Offset the adjacent faces to the desirable distance.
- Split the faces using the offset surfaces.
- Use Delete Face (Surface) to delete the split faces.
- Create a Surface Loft to cover the opening.
- Stitch the surfaces back to a solid body.
If it does not work, please share the f3d file here. The forum experts can help take a look.
Many thanks!
Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer
Start by extruding one section and chamfering one edge:
Repeat for the second circle:
Extrude the outer ring and combine with the other two bodies
Chamfer it:
Repeat the process for the other three openings.
ETFrench
Actually, it's better to do both sides of one circle, then pattern that. Add the outer ring and chamfer it:
ETFrench
@laughingcreek wrote:
this geometry should chamfer without any problem if it is properly made. before going to any great lengths trying to do this with any of the suggestions here just to hack a chamfer onto it you should post your model (export a .f3d and attach). even if you are able to hack your way into getting a chamfer, if the geometry is subpar, you're likely to continue to run into issues in other areas. understanding and fixing the underlying geometry issues would be be better.
I should save this as a text block 😉
@etfrench wrote:
The sharp angles in this design are blocking the chamfer operation. Try it.
I did of course-
@etfrench wrote:
... Try it.
Neither you nor the OP attached a model 😉
I'd love to take a stab at it. If it really doesn't work - not doubting your observation - then there might be yet another bug to report.
Thanks! It works fine in your model 😉
It isn't unusual, though, that a different but valid combination of steps or just different dimensions make Fusion cough hard.
The amount of overlap between the circles determines if the triangular opening will chamfer. When it is close to the center to center line, if fails:
When it's further away it succeeds:
ETFrench
I don't think the issue is with Chamfer.
I think the issue is a matter of user logic - the Chamfer is not going to end the way you expect it to.
The circles in the image below represent where the edges of the Chamfers would be on this face at this size.
On another note: I would never have repeated dimensions in sketch like this - look for symmetry and apply to Bodies/Features.
@TheCADWhisperer Thanks! I clearly did not have my thinking cap on 😕
Usually when filleting/chamfering starts to create problems, I start with a very small fillet. If that succeeds I increase the size and see where it starts failing. I omitted that here as well 😕
One solution, however has already been posted by @etfrench. The red circled area has the chamfer "fade out". More work, but a very nice solution!
One possible solution attached.
I am not completely satisfied with this one - but it should give you some ideas.
Notice simplified sketch...
with a bit more effort I think it could be made fully parametric in that it would not break with (reasonable) edits.
I would just keep it simple like in the attached. this method is strait forward and the chamfer isn't sensitive to the thickness of the rings. the rings do overlap (which is why it works) instead of touching tangent to each other at their outer diameter, bit perhaps it will still work for you.
