Getting started using gschem and spice-noqsi to simulate circuits in ngspice

This tutorial assumes you know how to draw circuits in gschem. If not, start with the gschem warmup. You'll also need some understanding of ngspice. There are several ngspice tutorials available, for example this one.

Here's a simple circuit, drawn in gschem. The symbols are standard gEDA symbols (vac-1, coil-1, capacitor-1, and resistor-1). The coil, capacitor, and resistor instances have value attributes attached. It also has a multiline toplevel attribute:

spice-epilog=
.control
ac dec 100 20k 500k
plot db(out)
.endc

The easy way to make such an attribute in gschem is to add it as text (AT). The only thing that distinguishes an attribute from ordinary text is the = sign, so if you enter the above, it functions as an attribute.

Having saved this as HelloWorld.sch, the terminal command:

gnetlist -g spice-noqsi HelloWorld.sch -o HelloWorld.cir

creates a SPICE circuit file from the schematic. Here's what HelloWorld.cir looks like:

* gnetlist -g spice-noqsi -o HelloWorld.cir HelloWorld.sch
* SPICE file generated by spice-noqsi version 20130710
* Send requests or bug reports to [email protected]
C1 GND out 1nF      
L1 1 out 1mH  
R1 GND out 10k      
V1 1 GND dc 0 ac 1

.control
ac dec 100 20k 500k
plot db(out)
.endc

Then, the terminal command:

ngspice HelloWorld.cir

shows this plot.

You'll have to type quit at the ngspice -> prompt to get back to the command shell. You could put this in the .control section above, but then it would just flash the plot at you and close it.

Finally, you can automate the command line operations with a Makefile:

HelloWorld : HelloWorld.cir
	ngspice HelloWorld.cir

HelloWorld.cir : HelloWorld.sch
	gnetlist -g spice-noqsi HelloWorld.sch -o HelloWorld.cir

clean : 
	rm -f HelloWorld.cir *~ \#*

With the Makefile, make or make HelloWorld will display the plot. make clean will clean up, removing the derived HelloWorld.cir along with temporary files gEDA tends to leave around.