WinSpice and Matlab: automation of electronic simulations

function [Rac Rtran] = spice_amp(x)
% Create the file .cir to be run by WinSpice3.
% Built-in function 'num2str' is used to modify parameters
% wherever it is convenient. 

b{1} = ['-------------Simple amplifier with Transistor----------- '];
b{2} = [' '];
b{3} = [' '];
b{4} = ['V1  Vin  0   dc 0   ac 1   sin(0 0.1 1e3) '];
b{5} = ['V2  Vcc  0   dc 30 '];
b{6} = [' '];
b{7} = ['R1  Vcc  b   10e3 '];
b{8} = ['R2  b    0   5e3 '];
b{9} = ['R3  Vcc  c   ' num2str(x(1))];
b{10} = ['R4  e    Vr ' num2str(x(2))];
b{11} = ['R5  Vr   0   1e3 '];
b{12} = ['R6  Vout 0   3e3 '];
b{13} = [' '];
b{14} = ['C1  c    Vout  10e-6 '];
b{15} = ['C2  Vr   0     10e-6 '];
b{16} = ['C3  b    Vin   10e-6 '];
b{17} = [' '];
b{18} = ['Q1  c    b     e     Q2N2222 '];
b{19} = [' '];
b{20} = ['.MODEL Q2N2222 NPN '];
b{21} = ['+(IS=3.108E-15 XTI=3 EG=1.11 VAF=131.5 BF=217.5 '];
b{22} = ['+ NE=1.541 ISE=190.7E-15 IKF=1.296 XTB=1.5 BR=6.18 '];
b{23} = ['+ NC=2 ISC=0 IKR=0 RC=1 CJC=14.57E-12 VJC=.75 '];
b{24} = ['+ MJC=.3333 FC=.5 CJE=26.08E-12 VJE=.75 MJE=.3333 '];
b{25} = ['+ TR=51.35E-9 TF=451E-12 ITF=.1 VTF=10 XTF=2) '];
b{26} = [' '];
b{27} = ['.control '];
b{28} = ['AC DEC 10 10 10MEGHZ '];
b{29} = ['write amp_ac_out.csv vdb(Vout) '];
b{30} = [' '];
b{31} = ['TRAN 10E-6 5E-3 '];
b{32} = ['write amp_tran_out.csv v(Vout) '];
b{33} = ['quit '];
b{34} = ['.endc '];
b{35} = ['.end '];
b{36} = [' ']; 

% Save file .cir line-by-line
[r,c] = size(b);
fp = fopen('amplifier.cir', 'w+');
for i = 1 : c
 fprintf(fp, '%s\n', b{i});
end
fclose(fp); 

% Run WinSpice
% Make sure wspice3.exe and .cir files are available in this directory
! wspice3 amplifier.cir 

% Read data saved in .csv files
% (assuming name termination _ac_out.csv and _tran_out.csv)
[Rac Rtran] = getWSpicedata('amp');

This is an important portion of additional code to read the .csv files.

function [Rac Rtran] = getWSpicedata(WSpiceBaseFile)
% Read csv files generated by a 'write' in a 'WSpiceBaseFile' (.cir file)
% Rac{1} = Frequency Points
% Rac{2} = AC response
% Rtran{1} = Time Points
% Rtran{2} = Tran response 

ac = fopen([WSpiceBaseFile '_ac_out.csv']);
Rac = textscan(ac, '%f %*f %f %*f', 'delimiter',',','headerLines', 1); 

tran = fopen([WSpiceBaseFile '_tran_out.csv']);
Rtran = textscan(tran, '%f %f', 'delimiter',',','headerLines', 1); 

fclose('all');

clear; clc; close all 

% We try some initial resistors
R3 = 1e3;
R4 = 50;
x = [R3 R4];

% Matlab launches the simulator including our parameters
[Ra Rt] = spice_amplifier(x); 

figure
semilogx(Ra{1},Ra{2})
grid on
figure
plot(Rt{1},Rt{2})
grid on 

% We try another gain modifying one of the resistors
R3 = 500;
x = [R3 R4];
[Ra Rt] = spice_amplifier(x); 

figure
semilogx(Ra{1},Ra{2})
grid on
figure
plot(Rt{1},Rt{2})
grid on