I am trying to create a 3D curve which is composed of a few segments of lines with radii between them (the lines are not lying in one plane). I connected the lines by creating the intersection points. But I couldn't find any fillet option for 3D lines?
I tried creating arcs between the lines. Although this was easy, but then I was stucked by trimming them, which was not easy at all.
Then I realised that there was a fillet line option which was under the sketch lines. But I couldn't find any 3D sketch option in NX. That feature (i.e. 3D sketch) is easy in Inventor (you can create 2D or 3D sketches).
My question is:
What is the simplest way to create fillets for 3D connected lines (say 3 perpendicular lines not in one plane)?
If the lines intersect, I'd use the old curve fillet command (found on the basic curves toolbar). Alternately, you can create an associative tangent arc between the lines and when you create the feature, use the "tangent curves" curve rule or the "follow fillet" selection option (no need to trim the lines).
If the lines do not intersect, use "circular blend curve" or "bridge curve".
Curves don't necessarily have to be trimmed, if you use the "stop at intersection" option, when creating your extrude, tube, revolve, etc.
I've done it with an assortment of sketches that were only the arc, before the "Circular Blend Curve" option. More than one roll cage was done like that.
"The fillet command exists only under the "sketch curve" command."
The fillet command that I mentioned can be found on the basic curves toolbar (menu -> insert -> curve -> basic curves...). The dialog is "old-school" so it may take some experimentation to see how it works. I like the 2 curve fillet option; pick each curve that you want to fillet/trim then pick the side that the arc center lies on. Note that the result will be unassociative.