Files

HSPICE Files

[ Introduction ] [ Files ] [ Source File ] [ Devices ] [ Commands ] [ Notes ]

HSPICE Input Files

source (netlist): filename.sp
design configuration: filename.cfg
initialization: hspice.ini

Note: The italicized files are those you must have.

HSPICE Output Files

run status: filename.st0
output listing: filename.lis
graph data, transient: filename.tr# (e.g. .tr0)
graph data, dc: filename.sw# (e.g. .sw2)
graph data, ac: filename .ac# (e.g. .ac1)
measure output: filename .m*# (e.g. .mt0)

Note: The italicized files are those that you will always have.

In general, you will only need to know about some of these files: source file, output listing, and graph data.

Source file (.sp)

The source file is your input file. This file contains your circuit description and all options and analysis you wish HSPICE to deal with. The structure of the file looks like this:

title			-Implicit first line, must be there

.options		-set conditions for simulation

ANALYSIS and TEMP	-statements to sweep vaiables

.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)

Note: This is just a suggested structure. Though the title always comes first and .end always comes last, the rest can come in any order in between. Another popular structure that is more implicit is to put the analysis statements after the circuit descriptions.

An example Netlist structure:

This is a source file		$must have a title line

.options post acct opts node	$HPSICE options



l6	6	16	.05	$indcutor 

c6	16	0	.05	$capacitor

r16	16	0	40	$resistor

c4	4	14	.1	$another capacitor

l5	data	15	1	$another inductor

c5	15	0	.2	$another capacitor



v4	4	0	dc 0 ac 0 0 pulse 0 1 0 .15 .15 .4 2	$voltage source

vdata	data	0	sin(1.0 1.0 1.0 0.0 1.0)		$voltage source

v6	6	0	exp(1 0.1 .02 .6 .2)			$voltage source



.model ...			$models and subckts



.tran	.1 5			$transient analysis

.print	v(6) i(r16)		$print statement

.plot	v(4) v(14) v(data)	$plot statement



.end				$Must have an end

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 (.lis)

This is one of the most important files in HSPICE as this file lists all results obtained from the simulation. This file contains (in order of listing in the file):

HSPICE licensing information
Listing of the circuit
Results form 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 data files are created by .OPTION POST command and contain the data to graphed by HSPLOT, AWAVES, or 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.

The material in this website is an expanded version of material presented by Dr. J. Steensgaard. This website is maintained by Shouri Chatterjee. This page was last updated on 02/11/2003