Circuit Simulator (WinSpice
and Matlab, improved interface)
In this
article, an improved Matlab
routine to drive the WinSpice circuit
simulator is
presented. This
method can also be easily adapted to
simulate and drive any circuit entered in SPICE.
The
concept of the Matlab
driver is illustrated by simulating a very simple RC lowpass
filter. In this
example
we're using Matlab ver. 7.0.1 and WinSpice3 ver. 1.04.07.
A first approach to the circuit driver was presented
here.
For more information about Matlab, visit www.mathworks.com.
For more information about WinSpice, visit www.winspice.com.
SPICE
stands for Simulation
Program
with Integrated
Circuit
Emphasis
Interchanging
information between Matlab and WinSpice allows
the
implementation of optimization algorithms and graphical
possibilities not included in the circuit simulator environment itself.
The
approach
developed now is very flexible and utilizes the inherent capability of
this SPICE simulator to include other circuit text files with
parameters, and print data
to external .csv (comma separated values) files.
First,
the circuit in Spice is defined (.cir file). This
circuit is simulated and tested within the WinSpice
environment
before
any attempt is made to interact with Matlab. We separate the components of
interest and include them in a different .cir file (using
the .include directive in the main file).
Second,
we prepare the output of the simulator by writing necessary data to an
external file, that is, we include 'write' commands in
the main .cir file, so that the results are saved as external
(.csv) text files
available to Matlab.
Third,
we now generate a version of the .cir file that includes
parameters using Matlab
capabilities
for manipulating strings. We then run the circuit
simulator from the command line.
After the simulation, we can read the results in the .csv files,
process them and act accordingly.
First Step:
We create, test and simulate this simple RC circuit in
WinSpice:
We initially use these values:
R = 10k ohms, C = 1 nF
The main .cir file (which is also a text file) is:
 RC
 LP filter 
V1
Vin 0 dc 0 ac
1
.include
param.cir
R vin
out {RES1}
C out 0
{CAP1}
.control
AC DEC
10 10 1MEGHZ
plot
vdb(out)
.endc
.end
The actual parameters are located in a separate file named 'param.cir',
which in this case only contains one line:
.param
RES1=10e3 CAP1=1e009
As expected, the AC analysis delivers this result (the cutoff frequency
is about 16 KHz):
Second Step:
We include appropriate 'write'
commands in the main .cir file, so that the results are saved as
.csv
files available to Matlab.
The control block changes into:
.control
AC DEC
10 10 1MEGHZ
write
RC_LP_filter_ac_out.csv vdb(out)
quit
.endc
.end
Third Step:
We now create a function (to be run by Matlab) that can
reproduce the secondary .cir file (including the
parameters), modify relevant parameters with the command 'num2str' (which
changes numbers into strings), and launch the circuit
simulator. This is the full code that accomplishes
it:
function [Rac] =
WS_RC_low_pass(x)
%
Create and save the file 'param.cir' to be included in
% another file to be
run by WinSpice3.
%
The builtin function 'num2str' is used to modify parameters
%
wherever it is convenient.
p = ['.param
RES1='
num2str(x(1)) '
CAP1='
num2str(x(2))];
dlmwrite('param.cir', p, 'delimiter','');
%
Run WinSpice
%
Make sure wspice3.exe and .cir files are available
% in this directory
!
wspice3 RC_LP_filter.cir
%
Read data saved in .csv files
%
(assuming name termination _ac_out.csv)
[Rac] =
getWSpicedata2('RC_LP_filter');
Compare the simplicity of
this code against the previously
developed code.
We eliminated the need to rebuild the complete
'.cir' file with Matlab, and we concentrate only on the relevant parameters.
There is an
important portion of additional code to read the .csv files.
function [Rac] =
getWSpicedata2(WSpiceBaseFile)
%
Read csv files generated by a 'write' in a 'WSpiceBaseFile' (.cir file)
%
Rac{1} = Frequency Points
%
Rac{2} = AC response
ac =
fopen([WSpiceBaseFile '_ac_out.csv']);
Rac =
textscan(ac, '%f
%*f %f %*f', 'delimiter',',','headerLines', 1);
fclose('all');
Now, we're ready to perform some simulations driving
WinSpice from Matlab.
clear;
clc; close all
%
We try some initial components
R1 =
10e3;
C1 =
1e9;
x = [R1
C1];
[Ra] =
WS_RC_low_pass(x);
figure(1)
semilogx(Ra{1},Ra{2})
grid on
%
We try another cutoff frequency by modifying the resistor
R1 =
1e3;
x = [R1
C1];
[Ra] =
WS_RC_low_pass(x);
figure(2)
semilogx(Ra{1},Ra{2})
grid on
For R1 =
10k and C1 = 1 nF, the obtained result is:
For R1 = 1k and C1 = 1 nF, the obtained result is:
As before, we can now use WinSpice as if it was another builtin Matlab
function! This
means that we can work through circuit optimization using functions
such as 'fminbnd'
or 'fminsearch'...
We
can try some numbers in our design, we can see the results and use
Matlab to modify relevant values in the circuit,
iteratively...
Reference:
http://desi.iteso.mx/erayas/cad.htm, 2014.

