"Failed to perform boolean operation" when sweeping or combine/cut from profile?

[Anonymous]

Hi Guys

I've encountered a strange one this morning. Im attempting to sweep this profile as a cutting operation around the top of this table top replicating a type of router bit we utilise at work. This would not work due to it first "intersecting itself" and now "boolean feature could not be created". A couple of times I attempted to create a new body then combine, cut, do not keep tools. The new body created, but then when attempting to combine, cut, do not keep tools it had the same error "failed to perform boolean operation".

Typically I would just use the lowest outer profile line of the top body as the path but it didn't seem to like it hence the offset line on the top im attempting to use.

The fillet at the corners would also normally only be 50 but have increased that durastically to try fix my problems to no avail.

I do these sorts of operations allllll the time but for some odd reason is failing for this one.

Any help would be much appreciated! 

[laughingcreek]

the sweep is failing at the halfway point of the table.  interestingly, the curvature comb of the path looks like this at that point-

this terrible curvature is being caused by 2 things-

1-offseting sketch splines frequently causes bad curvature in fusion. (work arounf is to extrude a surace, offset the surface, and use the edge of that instead. curvature quality will be better.)

2-the tangent constraint shown here was applied to the vertical line.  there is a microscopic curve right at the end of the line. (the tangent handle is actually very small and vertical here.  that's why you cant see it. delete the tangent constraint and just make the tangent handle horizontal instead.)

[Anonymous]

hi there thanks for helping me here. I have removed the tangent constraint, and made the handle horizontal but still no luck! Still problems around that midpoint

[laughingcreek]

most likely there are still problems with the splines. (can't say, you didn't attach a new file).  using mirror or symmetry on splines is difficult because certain changes don't automatically get reflected in the other splines. 

one way to avoid that is to not use symmetry/mirror on fit point splines.

see attached.

I also moved the profile in off the edge .5 mm because it wasn't fully cutting thru every where.

[Anonymous]

You were dead right, there was a whole mess of things going on at that vertices at the mirror line. Started again and good to go. Secondary question, what was that curvature comb thing you had going on in your earlier post??

[laughingcreek]

curvature combs are  useful tool when doing anything with curves or when surfacing.  for sketch curves, you can turn them on from the sketch pallet, and for body edges you use the tool under the "inspect" tab.  I suggest googling them and learning how to use if you haven't already.