can not make a filet

[Anonymous]

can not make a filet 

[laughingcreek]

It's hard to say with out the file.  Have you tried clearing the yellow error on the loft?  occasionally those will prevent things from working.

post your file if that' not it.

[Anonymous]

how do you post a file?

[laughingcreek]

from the file menu, export a fusion arhive file (.f3d) and attach to bottom of post

[Anonymous]

here is the file

[laughingcreek]

I'm at a loss as to why the "constant radius" fillet can't be made bigger than .05.  You can change the fillet type to "cord length" instead (a better fillet type for this type of situation anyway) and get a much larger fillet.

[Anonymous]

actually i trying to make a smaller filet like .12 

also you can not thicken the part .

[laughingcreek]

I guess you could make it a solid and shell it.  have to do the shell before making the visor though, which may not work for what your trying to do.  here's a screen cast of what I mean.  you can also do the fillet with this method. 

[laughingcreek]

never mind.  you can do the visor before shelling.

[Anonymous]

Thank you for showing me a at another way to do it . below is link from the autodesk design Academy 

https://academy.autodesk.com/curriculum/f1-schools-helmet-design

Fusion 360 Adding Detail to the F1 Helmet Part 2.mp4  from frame 5.26

i follow they they instruction . and they where able to do it . 

[jeff_strater]

I took a look at this helmet design.  I agree with @laughingcreek that there are better ways to design this helmet, and those videos are good examples.  But, I looked at the design as you had created it, and I understand why the fillet has problems.  It all goes back to the surface created by the loft.  There is a lot of bad geometry in part of that surface.  You can help this a bit by adding rail curves to help guide the loft.

screencast:

Jeff

[jeff_strater]

found something interesting while trying to track down the reason that loft feature was showing an error.  If I re-create that loft, I get different (better) geometry, and can apply the fillet:

very strange...

[laughingcreek]

@jeff.strater-

Funky geometry? yes.  Because of the loft? No.  I ran into this problem a while back, and couldn't get an answer then either.  But I have since stumbled across the solution.  Don't know why I didn't realize it applies to this case also.

The problem originates with the T-spline.  Geometry around the star points is always a little wonky.  Making a cut to close to one creates an edge that is problematic to loft from.  And it can be hard to see.  The solution is to further subdivide the area on the original t-spline before cutting it.  This gives a better edge that creates a better loft.

(I just did the one t-spline body in the OP's file, but should have done both.  Also, I didn't look at the lesson the OP was working from, but if his file is a true representation of the intended workflow, it's full of bad advise on how to get a good model.  That might should be looked at also.)

[laughingcreek]

just saw your follow up post jeff, we're tripping over each other.  I still think the t-spline body is originating this issue.  You get nice clean edges if you subdivide both surfaces before cutting.

[jeff_strater]

@laughingcreek, you are probably correct.  I didn't trace it back to the TSpline, but that makes sense.  Your solution is better!

Jeff

[laughingcreek]

Just want to drive this home.  Recall I subdivided the outer shell, but not the inner shell.  Here is what the curvature combs look like.  As you can see, there is the tiniest little bit of jigger still on the cut edge for the inner shell.  This is enough to screw up surfacing commands, and close to impossible for someone to find unless they know to go looking for it.

It would be good if fusion were robust and smart enough to know that a little kink in an edge, that isn't even visible, needs to be dealt with.  maybe a setting in the dialog boxes to smooth such things that would work similar to the tolerance setting in the stich command.  At least highlight the point of failure for goodness sake. 

[Anonymous]

thx every body for helping me

. i redesign the helmet as a solid model . can still not make a filet .

i imported the fusion file in solidworks . from there i was able with no problem to make two .12 fillets with no problem . 

than re import the file in fusion and the filet are fines .

must be a bug in the software . 

but thank again for the help .today learn How , to use the Project /include intersect . 

and to use the curvature comb 

also i could not figure out out to insert a screen cast inside this  reply .

[Anonymous]

here is the screen cast