Cool! Also you can quickly create 3d lines (i.e. off the sketch plane) in the same sketch by various methods. For example, if you tilt your view at somewhat of a low angle, then try making a line from a point, should get this triad as shown below, which allows to draw the line in 3D directly:

The method I'm using above is to create reference geometry in the sketch plane to then make 3D vertical lines from, since trying to control angles and dimensions in 3D directly is more difficult. I then made most of the vertical lines construction geometry and connected their 3D end points.

You can also use the move tool to move existing sketch lines and points off plane.
Regarding the modeling/feature fillet tool, for various reasons whenever possible it appears better to use this, say for the edges or corners of an extruded object, instead of trying to make the fillets in the sketch (although for your case of making a path for sweep, pipe etc. this doesn't apply). I don't have the thread off hand, but here is some text from it regarding some reasons to prefer this fillet approach:
"This is a great discussion around best practices in modeling. I certainly advocate for not putting fillets in sketches whenever possible. That's not to say "never", for instance if part of the design intent in the sketch requires a fillet then by all means put them in the sketch. If, however, the filets are only secondary or tertiary level of detail/transitions required for manufacturing, I almost exclusively use fillets as features rather thank sketch entities. Two reasons:
1. In the event that you find yourself working with a problematic model, the simpler the feature set that defines the geometry, the easier it will be to diagnose and fix any problems. Sketches should be distilled down to be as simple as possible, the definition of "simple" is entirely up to the designer or the standards set by a company. This principle helps reduce the burden of corners <pun> one can paint themselves into in a parametric modeler (this is not unique to Fusion; Inventor, PTC, Solidworks, etc. all can support poor modeling practices that end up with a model that can become riddled with problems and errors). A very simple illustration of this is say I have a shelled part, the primary shape is built from a sketch with all the fillet details necessary to create my finished plastic part design. If that shell fails to meet the requirements of the thckness that you as the user needs to determine "where" that failure is occurring. Experience tells me that the failure will likely be in the radii of one or more of the fillets. now I have to edit my sketch to find the problem and the potential for downstream features to be compromised greatly increase and you'll often end up "hacking" the modle to get it to just work so you can move on.
2. If you are working on somebody elses model and need to "fix" a problem area or add additional detail, say add some reference to a theoretical corner that is filleted, if that geometry exists in the sketch, but not the model, It's pretty easy to make the necessary reference. If your collaborator adheres to this modeling principle then your job can get done much faster and subsequent users won't be looking at "hacky" models."
I've seen other reasons as well, but don't remember off hand.
Again post with any other questions!
Jesse