How can I surface fill a three sided object that goes to a single point

[Anonymous]

I'm pretty new to fusion 360. Been trying to figure out the order of operation with the loft command. I've been mildly unproductive trying to figure it out for the last three hours. Is it possible to do a surface fill a three-faced object converting to a single point? or any other kinds of fill?

This is all I've managed to achieve so far. I either get just a general conflict error or rail is not smooth error.

Any help would be appreciated.

[davebYYPCU]

If it is symmetric, only do one half.

Make sure the two points at the nose are snapped together.

Loft half the base shape to the centre line and use 2 rails (the mid sketch and tall sketch).

Need the file for a better assessment.

[Anonymous]

I was trying what you were saying It worked once but I got the "path not smooth" error on the other half and now I just get the "path not smooth" error for both sides.

All points seemed connected.

Here's the file.

If it works for you please let me know what order you did it in.

I appreciate the help.

[davebYYPCU · Accepted solution]

I got the red dot error at the nose, so rebuilt the intersecting point at the nose.  I found 2 points there and had to delete one, but I may have built the second point myself, either way, one point there and the 

suggestions I mentioned, works fine, in any order now.

Loft on the other side with the same inputs works as expected.

Might help....

[Anonymous]

I'm at a loss.

Is there some kind of setting that would be causing this?

As soon as I add the first rail "Rail to Smooth" happens.

[Anonymous]

I finally found the extra point, deleted it, and rebuilt the end. not sure why I didn't find it the first time I checked for it. Thanks for the help I appreciate it.

[davebYYPCU]

I just finished a second review - pleased your are sorted.

Will ping @jeff_strater to add this to the list.

[chrisplyler]

I'm only guessing here, but...

I suspect that "too smooth" is misleading. I suspect it may be caused by a near tangency...something that can happen when you eyeball a connection but it ends up being a 0.0007413 degree corner or something like that, where it really should have a tangent constraint that will force it to be a smooth transition from one line to the other. Fusion seems to have trouble with all kinds of operations when a near tangency exists.

[davebYYPCU]

Actually - from the method to fix the problem - its likely a conflict between the sketching Constraint system, and the criteria required by the Loft system.

The File as supplied should work and doesn’t.

Sketch 8 Delete the centre line for clarity.  Hover over the nose end point, no coincident icon shows up.  Select Other in that area shows the spline, and 2 points.  Those 2 points are not viewed as coincident.  When you rebuild the point intersected from Sketch 6, and make the spline coincident to it, Loft works, and the coincident icon now shows up.

Rule no 1 for Lofts - intersections must be coincident connections.

Granted I have seen the near Tangency problems, too but not this time, 

Sketch solver doesn’t think they are coincident,

The error message about a Rail is - just - I gotta say something, - but there is no rail involved here just 2 profiles.  ( 2 Profiles that don’t connect is a legitimate Loft any day)  

My opinion, Loft was finding a self intersection, until the points are known to be coincident.