1. Input File

HSPICE input is composed of (mainly) four part.

1.1. Title line

Title line is always the first line of the input file. HSPICE simply neglects it. Since this line is echoed back in the outputfile for the page header, it is a very good place to describe what this simulation is for. This line is required, so make sure not to put an actual netlist element there, as it will be ignored by SPICE

1.2. Element description

Will be discussed in more detail later.

1.3. Control lines

Command lines that you use to control the behavior of HSPICE.

1.4. .END

Anything after the .END line is ignored.

* Comment

Any line starting with * is considered as a comment.

* Line continuation

Any line that starts with + sign is considered as the continuation of the previous line.

2. Element Description

2.1. Active device

2.1.1. MOS

Any line that starts with M is considered as the description line for a MOS transistor.

MXX Node_D Node_G Node_S Node_B MODEL_NAME
+ W=W_VALUE L=L_VALUE [AD=AD_VALUE] [AS=AS_VALUE]
+ [PD=PD_VALUE] [PS=PS_VALUE]

W, L : Width and Length of MOS
AS, AD : the area of the source, drain region(optional)
PS, PD : the peripheral length of source, drain region

You will need to specify AD, AS, PD, and PS if you are concerned about the parasitic capacitances of the drain and source area.

(Example)

M100 4 1 3 3 NCH W=10u L=1u AD=30p AS=30P PD=16u PS=16U

defines a MOS transistor named M100 with its drain connected to node 4, gate to 1, source and bulk to node 3. Its width is 10, length 1 micron. Area for the source and drain are 30*10E-12, and their peripherals. Now since the model is NCH, you need to define its model. The simplest for of MOS model definition would be :

.MODEL NCH NMOS

The above line tells you that the mos type NCH is a NMOS device. It doesn't say anything more than that, so you may want to, at least, add its threshold voltage.

MODEL NCH NMOS
+ VT0 = 0.7 ...

For the model parameters, refer Textbook P. 185 ~ P. 187.

2.1.2. Bipolar transistor

QXX N_Collector N_Base N_Emitter MODEL

2.1.3 Diode

DXX N_anode N_cathode MODEL

2.2. Passive Device

RXX N1 N2 Rvalue ---- Resistor
CXX N1 N2 Cvalue ---- Capacitor
LXX N1 N2 Lvalue ---- Inductor

2.3. Independent source

There are two types of independent source, voltage source and current source.

2.3.1. Pulse

Most frequently used time-varying waveform is a pulse. For example, a line like the following:

V1 10 11 pulse 0 5 10n 1n 2n 4n 10n

says that there's a voltage source connected between node 10 and node 11, which toggles between 0V and 5V, with leading time (delay) of 10n, 1ns rising time, 2ns falling time and 4ns high time, and period 10ns.

Be careful, however, if you write

V1 10 11 pulse 5 0 10n 1n 2n 4n 10n

now the 1ns is falling time, not rising time since V1 is originally 5v instead of 0V.

2.3.2. PWL

PWL is used for piecewise linear waveform. Most flexible, but need many parameters to use.

VNAME n1 n2 pwl t0 v0 t1 v1 t2 v2 t3 v3 ...

The value of VNAME is v0 at t=t0, v1 at t=t1, and so on.

2.3.3. Sine

Sin is for sinusoidal waveform.

V1 10 0 sin v_off v_amp freq [phase]

v_off is offset value, v_amp is the amplitude, freq is the frequency

2.4. Dependent source

Dependent sources are very useful elements in HSPICE. The four kinds of inear dependent sources are :

VCCS : voltage-controlled current source (G element)
VCVS : voltage-controlled voltage source (E element)
CCCS : current-controlled current source (F element)
CCVS : current-controlled voltage source (H element)

They are described in the following form.

GXX N+ N- NC+ NC- Gain
EXX N+ N- NC+ NC- Gain
FXX N+ N- NC+ NC- Gain
HXX N+ N- NC+ NC- Gain

3. Analysis

3.1. DC analysis

When you want to perform a DC analysis, you use the .DC control line. Its format is

.DC VARIABLE start_value stop_value increment_value

HSPICE will step throught the VARIABLE value start from the start_value in increment of increment_value until the VARIABLE reaches the stop_value.

Associated with any .DC control should be a .PRINT or .PLOT control line which will cause an output to be written to the HSPICE output.

3.2. AC analysis

.AC LIN n_point fstart fstop
.AC DEC n_point fstart fstop
.AC OCT n_point fstart fstop

HSPICE calculates the operating condition, and form a small-signal equivalent circuit for the given netlist. Then it performs ac analysis. You need to have at least one AC independent source. The frequency of any AC source in the circuit is set to fstart. The frequency increment value is defined by the increment option. If LIN is used, frequency is sweeped from fstart, and ends when frequency = fstop. Total number of frequency points used in this simation is n_point. If DEC is used, there are going to be n_point points within one decade, and there are n_point points within one octave if OCT is used.

Associated with any .AC statement should be a .PRINT or .PLOT or .PROBE.

Suppose you have a simulation setup like the following :

Vin 1 0 DC=1 AC
.AC DEC 10 10 100MEG
.print ac vdb(10) vp(10)

Then HSPICE will print out the voltage at node 10 with various frequency from 10Hz to 100MegHz in decibel scale. It will print out the phase of node 10, too.

If node 1 was the input for the circuit, then the printed output Vdb(10) will be the gain of your circuit from node 1 to 10. Since 'DEC 10' is used, there will be 10 points (in log scale) within each decade.

3.3. Transient analysis.

.TRAN t_increment t_stop

HSPICE will start simulating the circuit from time 0 to t_stop. The internal timing step is adjusted automatically to get the required accuracy. Parameter t_increment is used for output printout. It is also used in the internal time-step control algorithm, so when a accurate simulation is required, use a smaller number.

3.4 TF analysis

....
VIN 1 0 3v
.TF v(10) vin
....

will print out the transfer gain from the source specified as vin to the voltage of node 10.

The value specified when vin is defined (3 volt in this example) is used for bias calculation.

4. Misc and Notes

Please use .OP control. .OP will print out the operating point information for each node, each voltage and current source, and each element. The output from .OP is very useful in understanding the behavior of each evices.

For example, if you have too little gain from simulation result, most likely some transistors are biased in linear region(MOS case). You can easily check this by looking at the gm of the transistors.