UNIVERSITY of
PENNSYLVANIA
DEPARTMENT OF ELECTRICAL ENGINEERING
Example of SPICE simulation of
mutual inductances
The syntax for a mutual inductance is as follows:
Kname Inductor1 Inductor2 value_of_K
In which K is the value of the coupling coefficient that determine the mutal
inductance: M=K.sqrt(L1xL2). An example of a complete SPICE file for the
circuit given below follows.
- Vin 1 0 sin(0 5 159.15 0 0)
- Rs 1 3 100
- Rl 4 0 500
- L1 3 0 10M
- L2 4 0 2M
- K L1 L2 0.693
- .TRAN 0.1M 10M
- .PRINT TRAN V(3) V(4)
- .PLOT TRAN V(3) V(4)
- .END
Remarks:
- SPICE always needs a reference node numbered 0. One can never leave any node floating. For that reason we have connected the two coils together to node 0 (or put a large resistor between it). As there is no current flowing through this section, the circuit will not change by connecting these nodes.
- SPICE does not allow to connect a voltage source in parallel with an inductor, as it thinks that the voltage source is short circuited. You can place a small resistor (ex. 0.001 Ohm) in series with the voltage source to overcome this problem.
Back to Spice Guidelines
Jan Van der Spiegel; jan@ee.upenn.edu
Created Sept. 30, 1995; Updated Feb. 8, 2007