Tiago Oliveira Weber

First we want to calculate the value of our resistors. Let us assume resistor R1 is 10k, and then calculate R2 in Octave:

#+NAME: design_variables
#+BEGIN_SRC octave :results drawer :exports both 

gain=-10;
r1=10e3;
r2 = -gain*r1;
ans = [gain, r1, r2];

What we have now is a vector with the gain and the resistor values. No rocket science on these calculations, but as we are using Octave or Matlab to perform them, you can see that sky is the limit for what we can do.

With the vector in a variable we will now use it in a spice netlist to be simulated on Ngspice.

#+NAME: ngspice_sim 
#+BEGIN_SRC spice :results drawer :exports both :var design=design_variables file="amplifier_sim"

*Opamp with resistor values calculated in Octave
vin in 0 ac 1 sin(0 0.1 100Hz) dc 0
r1 in inn $design[1]
r2 inn out $design[2]
*EOpamp out 0 0 inn 1000
xamp1 0 inn vdd vss out lm741/ns
vdd vdd 0 5
vss vss 0 -5
.include spice_library/LM741.MOD
*.tran 0.1ms 0.05s
.ac dec 100 1 100e6
.end
.control
run
set gnuplot_terminal=png
let gain = v(out)/v(in)
meas ac gain_dc find gain at=1
meas ac gain_at_100k find gain at=100k
echo "$&gain_dc,$&gain_at_100k" > $file.txt 
gnuplot $file vdb(in) vdb(out)
.endc

-9.99943

-4.32609

The simulation had 2 measurement outputs (the DC gain of the circuit and the gain at 500 kHz) and one image (the input and output over frequency in dB). The important thing to notice here is that you can produce multiple outputs. The $file is an important variable on ob-spice because it tells the extension where to look for the results. For textual outputs, you should use "echo" to generate comma separated values based on measurements and output them to $file.txt, like the example below:

echo "$&var1,$&var2,$&var3" > $file.txt 

For plot, you use "gnuplot $file signal_names":

gnuplot $file vdb(in) vdb(out)

You can check the ngspice manual for more information on how to use ngspice commands.

We will now get the results from the simulation back to Octave in order to calculate the error between ideal and simulated.

#+NAME: error_calculation
#+BEGIN_SRC octave :results drawer :exports both :var gain_octave=10 ngspice_results=ngspice_sim[0]

gain_octave = design_variables(1);
gain_ngspice = str2num(gain_ngspice)
error_absolute = abs((gain_octave-gain_ngspice))
error_percentage = abs(error_absolute/gain_octave)
ans = [error_absolute,error_percentage];

And voilà, you have now your DC gain error calculated.

You can present the result directly in your text with an inline code-block or in fancier approaches, like creating a table as below (where I used python to print the results).

#+BEGIN_SRC python :results output drawer :exports results :var vi=design_variables ngspice_sim_var=ngspice_sim[0;0] error_calculation_var=error_cal

print "|-------------------------+--------|"
print "|                         |Gain    |"
print "| Ideal (specification)   |%.5f V/V|" %float(vi[0][0])
print "| Simulated (Ngspice)     |%.5f V/V|" %float(ngspice_sim_var)
print "| Absolute Error (Octave) |%.2g    |" %float(error_calculation_var[0][0])
print "| Relative Error (Octave) |%.2g %% |" %float(error_calculation_var[0][1])
print "|-------------------------+--------|"

The possibility to perform calculations in Octave or Matlab, simulate circuits based on these calculations on Ngspice and take the results back to Octave again all in the same text editor is incredible. When you add up the fact that this same customizible editor can export to most of your favorite formats like pdf, html, tex or txt, what you have is a designers's heaven. Of course there are lots of missing gaps that you won't be able to fullfill only with emacs. For instance, you won't be able to create a PCB layout in emacs, but org-mode can make it incredibly more easy to manage all your files, even the ones you can't directly treat with emacs.