Using ngspice to simulate a zener diode 2015-11-28
Electronics
1 Comment

In this post, I will demonstrate one of my earliest experiments in using SPICE for simulating a zener diode. In my previous post, I talked about my history with power electronics and how I am beginning to use circuit simulation to get a better handle on what is going on.

First off, I am using ngspice. Here is all you need to do to install ngspice on Ubuntu 14.04:
(from a terminal)

sudo apt-get install ngspice ngspice-doc

Fortunately for us, ngspice is in the Ubuntu multiverse repo.

Now to run it, you need to save this to a file called zener.cir:

Simple zener diode test
*
* A simple zener diode test circuit
*
vin vcc gnd SIN(0v 24v 50Hz)
dbridge mid vcc DMOD
rload mid gnd 100
*
.model DMOD D(bv=12v)
*
.end

The first line is the description of the circuit. The “.tran” line says we will simulate the circuit every 10 microseconds for .2 seconds.

For the circuit description, the “vin” object connects two points on the circuit named “vcc” and “gnd” and it is a sinusoidal 24V 50Hz power source. “dbridge” is a diode (using model DMOD below) whose positive side is at a point called “mid” and whose negative side is at “vcc”.  “rload” is a 100ohm resistor connecting “mid” to “gnd”. The “DMOD” line is a diode model with a breakdown voltage of 12V. 

Here is the basic schematic of this circuit:

To run it, simply type:

ngspice zener.cir

and then from the ngspice prompt, type:

run
plot v(vcc,mid) vcc

If you’ve done all of the above steps properly, you should now see a window with the following plot:

You can see the diode reverse voltage (vcc->mid) in red, and the vcc sinusoidal voltage of the power supply in blue. Notice how the diode voltage breaks down at 12V. To plot the voltage across the resistor you could do:

plot mid vcc 

This results in the following plot:

Now feel free to tinker with the file and make adjustments. Once you’ve made your changes and saved it, you don’t need to re-run from the beginning. Just type something like the following:

source zener.cir ; run; plot v(vcc,mid) vcc 

As one final note, there is a trick I’ve seen in many places to measure current. Basically, since power supplies in ngspice allow you to measure their voltage as well as current, you can create a 0V power supply anywhere in your circuit and use it to measure current. Here is a modified version of the above with a 0V power supply called “vmeas” bewteen “vin” and “dbridge”:

Simple zener diode test
*
* A simple zener diode test circuit
*
.tran 10us .2s
*
vin vcc gnd SIN(0v 24v 50Hz)
vmeas vcc top 0V
dbridge mid top DMOD
rload mid gnd 100
*
.model DMOD D(bv=12v)
*
.end

Make the changes to your file, save it back out (to the same filename zener.cir) and now you can use the following commands to reload and plot the current:

source zener.cir ; run
plot i(vmeas)

That’s it.

For my next post on this subject, I will try to demonstrate (my first foray into) how to use ngspice to model a MOSFET based on a datasheet.

If you try any of this out, please send me a comment to say how it worked for you!