How to know phasor current direction in LTspice AC analysis
The convention in SPICE world is that two pin elements have a unique direction of current, from pin 1 to pin 2. For 3 or more pin elements, the current is always considered going into the pin.
In the link you posted they are using custom symbols, something stated right in the opening paragraph (top of the page):

In addition to LTspice IV, this tutorial assumes that you have installed the University of Evansville Simulation Library for LTspice IV. This library extends LTspice IV by adding symbols and models that make it easier for students with no previous SPICE experience to get started with LTspice IV.

If you are using only the default library, hovering the mouse over the elements will cause the mouse cursor to change into an ampmeter, signaling the direction of the current, but this is no longer valid for a one point .AC analysis.
So the only way to make sure you know the direction of current beforehand is to be careful when you rotate the element: Ctrl+R will always rotate it clockwise. When the component is &quot;in your hand&quot; (i.e. not yet placed) it will have the 1st pin above and the 2nd below. If you place the components to always be (for example) from top to bottom, and from left to right, you will always know how the current will go through any branch. The order for the positioning doesn't matter as long as it's consistent, but as I described it makes it coincide with the convention of the currents through the wires in the schematic: from top-left to bottom-right.
One minor exception is the inductor which has in its properties (RClick) a check box that says: Show Phase Dot. That will always point to the 2nd pin.