Lofting error "rails do not intersect all profiles" but says its coincident

[gd0g4277]

Hello,

First off i've only been using fusion for about a week so im pretty green.  I'm trying to create a loft with 2 profiles and 4 rails.  I successfully created a loft with 3 profiles but keep getting error "rails do not intersect all profiles.  I 3d projected my sketch and im trying to make a rail from the purple line to another rail.  It looks like its snapping to the profile just fine and says its coincident but if I zoom in its a few thousands off.  What am I doing wrong?

[wmhazzard]

Sketch your rails last and use the intersect tool in the sketch environment to get the rail to intersect your profiles. If you sill can't figure it out, attach an f3d file of your model. 

[gd0g4277]

Thank you for the response.  I tried with the intersect tool and still got the error.  Here is the file.  This is only my third ever model and first in fusion so hopefully its not too much of a mess lol.

[davebYYPCU · Accepted solution]

The error is correct.

Your last Loft has 2 profiles, 

all - ALL four rails must connect to both profiles, you have Rail 4 connected to Rail 1.

You can’t do that.

Might help......

[gd0g4277]

This helped a lot.  I didn't fully understand how the profile and rails worked until you just said that and it clicked.  Thanks Dave

[gd0g4277]

Ok now that I have that fixed i've ran into another issue.  It wont let me thicken.  I keep getting this error. (Pic attached)

[TrippyLighting]

We need to see the current model.

1. How much do you want to thicken it?

2. Does that create self intersecting geometry due to too small radii?

This is not an object I would design with lofts, I'd use T-Splines. 

[gd0g4277]

Wanting to thicken .09375 inches (3/32). I lofted a t spline with the same result. The reason I’m lofting this is because there’s a certain bottom curvature in this model that needs to be exact for this part to fit correctly(I’m pretty ignorant on t splines as I’ve never really used the feature yet).  If I unstitch and try to thicken separately, it lets me thicken the back smaller section but not the front. I will upload the file when I get off work. Thank you for your time

[gd0g4277]

Here's the file for it. 

[TrippyLighting]

I created a section cut and sketched a circle with the thickness you specified as the diameter. As can be seen, the circle  does not fit in that small crevice. This is an indication  that when offsetting, thickening or shelling it would create self intersection surfaces, which Fusion 360 does not permit for good reasons.

You also are lofting into two singularities (circled in red).

[gd0g4277]

Thanks Peter.  Looks like I will need to smooth my loft more then?  Also on the singularity's, this is only half of the model.  I planned on mirroring it to create the full model.  Is that not possible with this geometry?