SPICE is a general purpose analog circuit simulator that is used to verify circuit designs and to predict circuit behavior. This is of particular importance for “integrated circuits”. It was for this reason that SPICE was originally developed at the Electronics Research Laboratory of the University of California, Berkeley (1975), as its name implies:
Simlulation Program for Integrated Circuit Emphasis
HSPICE is a commercial and very powerful version of SPICE that has fewer bugs than the freely avaliable Berkeley SPICE. HSPICE is a relatively comprehensive program that can be used to simulate very large circuits comprising many different types of components. HSPICE is able to handle hierarchical circuit structures (i.e., you can define subcircuits) and supports both local and global variables/parameters.
Circuit analyses supported by HSPICE:
Non-linear DC analysis: calculates the DC transfer curves from any input to any output.
Non-linear transient analysis: calculates the voltages the currents as a function of time when a signal is applied.
Linear AC Analysis: calculates the frequency response from the input to all specified node voltages and currents. Bode plots can be generated using a graphical post processor, such as AWAVES.
Noise analysis
Sensitivity analysis
Distortion analysis
Fourier analysis: calculates and plots the frequency spectrum
Monte Carlo Analysis
Components supported by HSPICE:
Independent and dependent voltage and current sources
Resistors
Capacitors
Inductors
Mutual Inductors
Transmission Lines
Operational Amplifiers
Switches
Diodes
Bipolar Transistors
MOSFET Transistors
MESFET Transistors
JFET Transistors
etc.
HSPICE - Files
HSPICE Input Files
source (nelist): filename.sp
design configuration: filename.cfg
initialization: hspice.ini
HSPICE Output Files
run status: filename.st0
output listing: filename.lis
graph data, transient: filename.tr# (.tr0)
graph data, dc: filename.sw# (.sw0)
graph data, ac: filename.ac# (.ac0)
measure output: filename.m*# (.mt0)
Source file (.sp)
The source file is your input file. This file contains your circuits description and all options and analysis you wish HSPICE to deal with. The structure looks like this:
1 2 3 4 5 6 7 8
title - Implicit first line, must be there .options - set conditions for simulation ANALYSIS and TEMP - statements to sweep variables .print/.plot/Analysis - set print, plot, and analysis variables .initial conditions - input state of system netlist - circuit descriptions (components, input sources) .model libraries - .lib and .inc .end - terminates the simulation (always add a newline character)
Design configuration (.cfg)
Configuration files are used by HSPICE, AWAVES and HSPLOT to describe the available terminals and hardcopy devices.
Initialization (hspice.ini)
The initialization file deals primarily with setting up HSPICE itself and has no need to be modified by users.
Run status (.st0)
The run status file is a transcript of what operations HSPICE performs on a source file. The file sometimes offers help when debugging as shows steps not preformed by HSPICE.
Output listing - important (.lis)
This is one of the most important files in HSPICE as this file lists all results obtained from simulation. This file contains (in order of listing in the file):
HSPICE licensing info
Listing of the circuit
Results from the analysis of the circuit (.op, .print, .plot, .measure, .ac, and .tran in order of their appearance in the source file)
Graph data files (.tr#, .sw#, .ac#)
Graph date files are created by .OPTION POST command and contain the date to graphed by HSPLOT, AWAVES, HSPICE. Basically these files retain the data to be graphed from the .lis file in a different graphing format.
Measure output (.m*#)
The measure output file hold the result from .MEASURE commands. These files are not very useful because the data is hard to read and already exits in a nicely formatted way in the .lis file.
HSPICE - Source File
The HSPICE source file consists of five parts.
Title statement: the first line is the circuits title; it may be anything, but not neglected.
Data statements: description of the components and the interconnections.
Control statements: tells SPICE what type of analysis to perform on the circuit.
Output statements: specifies what outputs are to be printed or plotted.
End statement: on the very last line: .END followed by a carriage return.
1 2 3 4 5 6 7
TITLE STATEMENT ELEMENT STATEMENTS . . COMMAND (CONTROL) STATEMENTS OUTPUT STATEMENTS .END
Comment statements: can be anywhere in the source file:
‘*‘ - indicates a full line comment
‘$’ - indicates and end-of-line comment
Continuation: ‘+’ - indicates a continuation of the previous line.
NOTATION
HSPICE notation is relatively simple. Both upper and lower case letters are allowed, but no distinction is made (HSPICE converts everything to upper-case characters before any interpretation is attempted).
The statements have a free format and consist of fields separated by a blank. Each line is interpreted as a separate statement.
All statements begining with a ‘.’ are commands (.OPTION, .PRINT, .AC, etc.)
Statements that begin with an alphabetic character are treated as elements, the first character determines the type of element:
R for resistors
C for capacitors
L for inductors:
D for diodes
Q for bipolar junction transistors
M for MOS transistors
V for voltage sources
I for current sources
G for voltage-controlled current sources (tranconductance amplifiers)
F for current-controlled current sources (current amplifiers)
E for voltage controlled voltage sources (voltage amplifiers)
H for current-controlled voltage sources (tranresistance amplifiers)
X for subcircuits (hierarchical circuit structure)
Topology Rules
Every node must have a DC path to ground.
No dangling nodes (all nodes must have at least two connections).
No loops of only ideal voltage sources and capacitors.
No nodes connected to only ideal current sources and inductors.
Naming conventions
Node Identification:
0 is ALWAYS ground
It’s best to start all node names (besides ground) with an alphabetic character.
HSICE units
f=1e-15
p=1e-12
n=1e-9
u=1e-6
m=1e-3
k=1e3
meg=x=1e6
g=1e9
t=1e12
Global Variables
Syntax
.global node1 node2 node3 : globally defined nodes
.global vbias vcc : globally defined sources
Usage
when subcircuits are included in the data file
assign common node name to subsircuit nodes
power supply connection of all subcircuits is often done this way:
.global vcc: connects all nodes named vcc (all circuits have a common node)
Essential globals are used most often for subcircuits, though they are great for sources. Notice that ground (node 0) always is a global node.
HSPICE - Devices
General Element Statements
The element statement specifies the type of element or independent source used. It has a field for the element name, the connecting nodes, a value for the component, and optional parameters.
General Form:
1
NAME node1 node2 ... nodeN <model reference> value <optional parameters>
NAME Specifies the type and name of element. The first letter in the name field identifies the element as a specific type, the remaining letters give the element a unique name.
node Specifies how the element is connected in the netlist.
value Gives the values of the element
Refers to the model when the basic element value does not provide an adequate description.
Used to modify existing values within a .model for this paricular element. In order to words a .model might have a temperature of 27 degrees when you what 40 degrees Centigrade.
.model Statements
.model statements allow extra device descriptions are required for accuracy. For instance, a .model statement can be used to give resistors operating temperatures, L and W values to MOSFET’s, or even insulator thickness on a capacitor. .model statements can be included any within the .lis, though they are usually placed before the netlist for convenience.
General Form:
1
.model mname modeltype<keyword=value>
mname The model reference name specified in the associated element statement.
modeltype Specifies the model type to be used, i.e., R for a resistro, C for a capacitor, and L for inductor.
.param Statements
.param statements allow the user to define local variables. The variables can be defined as values, equations, or even functions.
General Form:
1 2 3
.param variable = 'expression' or .param variable = value
variable Represents the name of the variable or function to be defined. expression Represents the value, equation, or function to be assigned to the variable.
AC AC resistance used in the AC analysis. default=Reff
C Capacitance connected from node n2 to bulk. default=0.0
DTEMP Element and circuit temperature difference. default=0.0
equation The resistor can be described as a function of any node voltage, branch currents and any independent variables such as TIME, frequency (HERTZ), or temperature (TEMPER)
L Resistor length. default=0.0
M Multiplier used to simulate parallel resistors. default=1
mname Model name.
n1 Positive terminal node name.
n2 Negative terminal node name.
R Resistance.
Rxxx resistor element name. Must begin with ‘R’.
SCALE Element scale factor for resistance and capacitance. default=1
Cxxx Capacitor element name. Must begin with an ‘C’.
C Capacitance in farads at room temperature.
CTYPE For capacitance, if C is a function of v(n1,n2),then CTYPE=0 else =1. The capacitance charge is calculated differently depending on the value of CTYPE.
IV Initial voltage across the capacitor in volts.
The rest can refer to resistor which the definitions are the same.
Note: Inductor is skipped since I don’t use it in my design.
Active
Diodes
Diodes in HSPICE can be anywhere from very complex realistic diodes to simple ideal ones depending on the circuit designer. In general all diodes will have a model name and be defined by a .model statement. Since most models are provided, .model descriptions will not be given in any detail. The diode element uses the following formats:
nplus Positive terminal name (arrow end) of the diode.
nminus Negative terminal name (line end) of the diode.
PJ Periphery of junction.
WP Polysilicon capacitor width (in meters).
LP Polysilicon capacitor length (in meters).
WM Metal capacitor width (in meters).
LM Metal capacitor length (in meters).
OFF Sets the diode initially to the off operation region (DC analysis). default=ON
IC Initial diode voltage.
The rest options can be refer to resistor.
BJT is skipped.
MOSFETS
MOSFETs are another device within HSPICE that requires a .model statement. The .model statement is required to define whether or not the circuit designer want to deal with a p- or n-channel device. The syntax for the .model statement is shown below:
1
.model mname NMOS <or PMOS> <parameters>
Only the model name and the NMOS (or PMOS) are required. The MOSFET transistor element uses the following formats:
NRD Number of resistance squares of drain diffusion. default=0
NRS Number of resistance squares of source diffusion. default=0
RDC Contact resistance on the drain. default=0
RSC Contact resistance on the source. default=0
OFF Sets the transistor initially to the off operation region (DC analysis). default=ON
vbs,vds,vgs
vbs: initial bulk-source voltage
vds: initial drain-source voltage
vgs: initial gate-source voltage
DELVTO Zero-bias threshold voltage shift. default=0
GEO Source-drain sharing selector (only use for ACM=3 in .model). default=0
Independent sources
General Form
In general, voltage and current sources in HSPICE can be very almost anything from simple dc sources to incredibly complex piecewise linear ones. The general form for both current and voltage sources are shown below:
tranfun Transient source function (i.e. PULSE, PU, SIN, EXP, PWL, PL).
Pulse Function
The pulse function can create either a linear rectangular or linear trapazoidal pulse with an initial time delay. The function also has user defined rise, fall, and high times. The functions are placed in the tranfun position listed above. The pulse function has the form:
v1 Initial value of voltage or current before the pulse.
v2 Pulse current or voltage value.
td Time delay for the start of the transient interval to the up ramp. default=0
tr Rise time. default=TSTEP
tf Fall time. default=TSTEP
pw Pulse width. default=TSTEP
per Pulse repetition period in seconds. default=TSTEP (transient timestep)
Sin Function
The HSPICE sin function can produce a sin wave input with user defined delay, magnitude and phase. Also, HSPICE can also produce exponentially damped sin sources.
1
sin (vo va freq td damp<pd>)
vo Wave offset.
va wave amplitude.
freq Wave frequency in Hz. default=1/TSTOP
td Wave time delay in seconds. default=0
damp Wave damping factor in 1/seconds. default=0
pd Phase delay in degrees (not radians). default=0
Exponential Function
The exp function produces an exponential with user definable rise time and fall time constants and delay values.
1
exp (v1 v2 <td1> <t1> <td2> <t2>)
v1 Starting voltage or current.
v2 Pulse value of voltage or current.
td1 Rise delay time in seconds. default=0
t1 Rise time constant in seconds. default=TSTEP
td2 Fall delay time in seconds. default=td1+TSTEP
t2 Fall time constant in seconds. default=TSTEP
Piecewise Linear Function
The HSPICE piecewise linear function is a collection of user defined pulses and steps. All plateaus and rise and fall times are also user definable. In addition, when moving between differing voltages or currents, the function will always proceed linearly.
repeat The start time for the function to repeat in seconds.
t1… The time value in seconds.
TD Keyword for the function time delay.
delay Actual time delay in seconds.
v1… Current or voltage values.
Note: each voltage and time come in pairs.
HSPICE - Commands
Commands or Control Statements to Specify the Type of Analysis
.op Statement
This statement instructs SPICE to compute the DC operating points:
voltage at the nodes
current in each voltage source
operating point for each element
In HSPICE it is usually not necessary to specify .op as it gives you automatically the DC node voltages. However, HSPICE does not give the DC voltages unless you have specified a certain analysis type, such as for instance .tran or .ac analysis (SPICE automatically does a DC analysis before doing a transient or AC analysis). Thus, if you are only interested in the DC voltages in HSPICE, you should specify the .op option, or the .dc option.
.dc Statement
This statement allows you to increment (sweep) an independent source over a certain range with a specified step. The format is as follows:
1
.dc SRCname START STOP STEP
in which SRCname is the name of the source you want to vary; START and STOP are the starting and ending value, respectively; and STEP is the size of the increment.
.tf Statement
The .tf statement instructs HSPICE to calculate the following small signal characteristics:
the ratio of output variable to input variable (gain or transfer gain)
the resistance with respect to the input source
the resistance with respect to the output terminals
.tf outvar insrc in which outvar is the name of the output variable and insrc is the input source.
.sens Statement
This instructs HSPICE to calculate the DC small-signal sensitivities of each specified output variable with respect to every circuit parameter.
1 2 3 4 5 6
.sens variable ``` ## `.tran` Statement
This statement specifies the time interval over which the transient analysis takes place, and the time increments. The format is as follows:
.tran TSTEP TSTOP <TSTART >
1 2 3 4 5 6 7 8 9 10 11 12
- `TSTEP` is the printing increment. - `STEOP` is the final time. - `TSTART` is the starting time (if omitted. TSTART is assumed to be zero) - `TMAX` is the maximum step size. - `UIC` stands for Use Initial Condition and instructs HSPICE not to do the quiescent operating point before begining the transient analysis. If UIC is specified, HSPICE will use the initial conditions specified in the element statements.
## `.ic` Statement
This statement provides an alternative way to specify initial conditions of nodes (and thus over capacitors).
.ic Vnode1 = value Vnode2 = value
1 2 3 4 5
## `.ac` Statement
This statement is used to specify the frequency (AC) analysis. The format is as follows:
.ac LIN NP FSTART FSTOP .ac DEC ND FSTART FSTOP .ac OCT NO FSTART FSTOP
1 2 3 4 5 6 7 8 9 10 11
in which `LIN` stands for a linear frequency variation, `DEC` and `OCT` for a decade and octave variation respectively. `NP` stands for the number of points and `ND` and `NO` for the number of frequeny points per decade and octave. `FSTART` and `FSTOP` are the start and stopping frequencies in Herz.
## Output Statements
These statements will instruct HSPICE what output to generate. If you do not specify an output statement, HSPICE will always calculate the DC operating points. The two type of outputs are the prints and plots. A print is a table of data points and a plot is a graphical representation. The format is as follows:
.print TYPE OV1 OV2 OV3 .plot TYPE OV1 OV2 OV3
in which `TYPE` specifies the type of analysis to be printed or ploted and can
be:
- DC
- TRAN
- AC
The output variables are OV1, OV2 and can be voltage or currents. Node voltages
and device currents can be specified as magnitude (M), phase (P), real (R) or
imaginary (I) parts by adding the suffix to V or I as follows:
- M: magnitude
- DB: magnitude in dB (deciBells)
- P: phase
- R: real part
- I: imaginary part
# NOTES
1. Know what to expect from the simulation before running it.
2. Simulation is NO substitute for THINKING.
## Other helpful hints
1. You can measure the voltage at any node, or the voltage between any two nodes.
However, you can only measure the current passing through a voltage source. To
measure a current through a branch, insert a dummy voltage source of value 0 in
the branch (like an ammeter) and measure the current through this dummy voltage
source.
2. To extract the data from the `.lis` file, have `.print` statements. Use
`.options ingold` so that the data is in the exponent notation. Just edit the
`.lis` file that you get to have the data suitable for MatLab.
