# A gentle introduction to Spice

22 Nov 2014SPICE is an indispensable tool for simulating integrated circuits. Here, however, we would look at the SPICE as a tool for developing embedded electronics. Simulation always brings in some sanity and confidence in the head of the designer. That is precisely the goal of this tutorial series. Sanity.

SPICE provides 4 basic analysis

**OP**: (Operating Point analysis) Determine the steady state operating point of the circuit under simulation. Example, this analysis helps determine the quiescent voltage and current of say, a transistor amplifier.**DC**: In this analysis, the source input voltage of a circuit is varied over a range (say from 1V to 5V) and the behaviour of the circuit is observed over this range. Example, this can help determine the range over which a transistor remains in linear mode.**AC**: The frequency of a voltage source is varied over a range of frequencies and behaviour of the circuit is observed over this frequency range. Example, this can help plot the frequency response of a RC filter**Transient**: This analysis helps observe the behaviour of a circuit over time. Example, plotting the response of a circuit to a pulse input

We would go over each of the above mentioned analysis with simple examples.

## Introducing OP and DC

Let's start with the simplest form of analysis: Operating Point Analysis. SPICE performs this analysis before performing any other analysis.

```
Resistor and Diode
R1 n1 n2 1K
D1 n2 0
V0 n1 0 DC 3V
.end
```

Save this file as `ckt1.cir`

. SPICE files are conventionally stored with the `.cir`

extension. Names of nodes in the circuit start with `n`

.
First line of the file is the Title Line, and the last line of the file should be `.end`

. The syntax for describing the basic components is as shown

Component | Syntax |
---|---|

Resistor | `R<name> <node 1> <node 2> value` |

Diode | `D<name> <anode> <cathode> <model name>` |

Voltage source | `V<name> <pos> <neg> DC <value> AC <value>` |

Inductor | `L<name> <node 1> <node 2> value` |

Capacitor | `C<name> <node 1> <node 2> value` |

SPICE understands that `1K`

is one thousand. Shown below is a description of the units SPICE understands.

SPICE Symbol | Value in Scientific Notation |
---|---|

T | 1E12 |

G | 1E9 |

MEG | 1E6 |

K | 1E3 |

M | 1E-3 |

U | 1E-6 |

N | 1E-9 |

P | 1E-12 |

F | 1E-15 |

Now, fire up `ngspice`

in a terminal and execute the following

```
ngspice -> source ckt1.cir
ngspice -> op
ngspice -> show d1
```

`op`

does the operating point analysis of the circuit; `show d1`

displays the operating point of `D_1`

.

```
ngspice -> show D1
Diode: Junction Diode model
device d1
model D
vd 0.676901
id 0.00232313
gd 0.0898203
cd 0
```

Similarily, you can try out

```
ngspice -> show r1
ngspice -> show v0
ngspice -> show
```

The last **show** command displays operating point of all circuit elements in the circuit. To perform a DC sweep analysis, run the following

```
ngspice -> dc v0 0V 5V 0.01V
ngspice -> plot v(n2)
```

The syntax for describing DC analysis is `dc v<name> <vstart> <vstop> <vstep>`

.This sweeps the voltage source from `0V`

to `5V`

in steps of `0.01V`

& plots the voltage at `n2`

for this sweep. This results in the plot shown below

While you are at it, try running the following

```
ngspice -> plot i(v0)
ngspice -> plot i(r1)
ngspice -> plot (v(n1) - v(n2))/10K
```

You might observe that `i(v0)`

works, but `i(r1)`

doesn't (`ngpice`

says *no such function as i*).
Apparently, ngspice only allows plotting current though independent voltage sources. The command `plot (v(n1)-v(n2))/10k`

effectively plots current through `R_1`

## Introducing TRAN and AC

**AC** analysis and **TRAN** analysis only make sense for circuits containing reactive elements (capacitors and inductors). For circuits containing purely resistors, diodes, transistors and current/voltage source (ignoring parasitic capacitive and inductive effects), you should only perform **OP** and **DC** analysis as the voltage and current for such curcuits would be time independent. Let us now simulate a simple RC filter.

Let's start off with *transient analysis*.

```
RC low pass filter
R1 n1 n2 1K
C1 n2 0 10nF
V0 n1 0 PULSE(-1 1 20US 0US 0US 100US 200US)
.end
```

Save the above circuit as `ckt2-tran.cir`

. The voltage source is a periodic pulse train. The syntax for specifying a pulse train is

`Vname N1 N2 PULSE(V1 V2 TD TR TF PW Period)`

, where

```
V1 = initial voltage value
V2 = pulse voltage value
TD = delay before first change fron V1 to V2
TR = rise time
TF = fall time
PW = pulse width
Period = time period of the pulse train
```

Now, run the following analysis

```
ngspice -> source ckt2-tran.cir
ngspice -> tran 1us 1ms
ngspice -> plot v(n2)
```

The syntax for running transient analysis is `tran <tstep> <tstop> <tstart>`

Finally, let us carry out **AC** analysis. The circuit for this analysis is the same as the one for transient analysis, except that the voltage source would be sinusoidal.

```
RC low pass filter
R1 n1 n2 1K
C1 n2 0 10nF
V0 n1 0 AC
.end
```

Save the above circuit as `ckt2-ac.cir`

. Recall that *AC analysis* is all about varying the input voltage frequency over a range. Since we are dealing with linear circuits, the frequency of voltage and current at all nodes and loops in the circuit would have the same frequency (at steady state). SPICE provides a variety of ways of sweeping through a frequency range

- linear sweep
- decade sweep
- octate sweep

We will just look at linear sweep. The syntax for specifying linear sweep is

`ac lin NumberOfPoints StartFreq EndFreq`

As an example,

```
ngspice -> source ckt2-ac.cir
ngspice -> ac lin 1000 1 1k
ngspice -> plot abs(v(n2))
```

I would probably write a follow up tutorial on spice whenever I borrow some time from my workplace. Hopefully, this one was useful enough!

Tweetcomments powered by Disqus