Hello Helmut.
Thank you for your advice. I was able to modify the transistor models
from the SPICE directive, or even better, by editing the model files
for the NPNs. The .STEP is a good suggestion when you wish to play
with a single parameter.
As for you question regarding S-parameters, I have included a netlist
that shows how to measure S11 and S21 for a simple two-port
(consisting of a single shunt resistor Rtest2port) which you can
substitute by your circuit. Then, you duplicate the circuit and
switch
the sources from the input to the output to "measure"S22 and S12.
Then you plot Vs11, Vs22, etc, which correspond to S11, S22¡
Once that is done you can go to the plot window, and plot various
quantities like the Unilateral power gain by clicking ADD TRACE and
then paste the expression for U in the window as
(((MAG(V(s21)/V(s12)-1))**2)/2/(((1-(MAG(V(s11)))**2-(MAG(V(s22)))**2+
(MAG(V(s11)*V(s22)-V(s12)*V(s21)))**2)/2/MAG(V(s12)*V(s21)))*MAG(V(s21
)/V(s12)) - Re(V(s21)/V(s12))))**0.5
(note that the square root is needed because LTSPICE takes 20log of
everything in the dB scale)
NETLIST TO MEASURE S11 and S21
==================================================================
* C:\Program Files\LTC\SwCADIII\CB_Files\FET_model.asc
V1 N001 0 0 AC 1 0 Rser=0 Cpar=0
R6 N002 N001 50
E1 N003 0 N002 0 2
R8 S11 0 1G
V2 N003 S11 0 AC 1 0 Rser=0 Cpar=0
R7 N002 0 50
E2 S21 0 N002 0 2
R9 S21 0 1G
Rtest2port N002 0 100
.ac dec 99 1G 300G
.backanno
.end
