Mutual Inductance is designated in a SPICE netlist by beginning the first word (label) of a new line with the letter "K". It is unique among the basic circuit elements in LTspice in that a schematic symbol is not used to represented it. Rather, it is placed as a line of text (SPICE directive) onto the schematic and passes directly to the netlist to be processed by the solver. Note that text placed onto a schematic correctly as a SPICE directive will appear black in color (a comment will normally appear as blue text). Schematic text can be switched between the two types by ctrl-right-mouse-clicking on it and selecting the desired type via a "radio" button.
Syntax: Kxxx L1 L2 [L3 ...] <coefficient> L1 and L2 are the names of inductors in the circuit. The mutual coupling coefficient must be in the range of -1 to 1.
For coupling between more than two inductors two form are possible. The line:
K1 L1 L2 L3 L4 1
is synonymous with the six lines:
K1 L1 L2 1 K2 L2 L3 1 K3 L3 L4 1 K4 L1 L3 1 K5 L2 L4 1 K6 L1 L4 1
LTspice recommends starting with a mutual coupling coefficient equal to 1 in order to eliminate leakage inductance that can ring at extremely high frequencies (if damping is not supplied) and slow the simulation. However, be aware that a mutual inductance value of plus (or minus) unity may lead to simulation difficulties if Skip-the-initial-operating-point-solution (UIC) is specified for the .tran command. Specifying a realistic resistance for each inductor "winding" (ctrl-right-mouse-click) will minimize this tendency. Note that when coupled inductors are used as transformer windings, individual winding inductances rather than turns ratios must be specified (inductance ratios should be proportional to the square of the turns ratios).