Getting Started With HSPICE

Index:

• General Info
• Files
  • Suffixes
  • Descriptions
    • input netlist
    • design configuration
    • initialization
    • run status
    • output listing
    • graph data
    • measure output
• Netlist Notation
  • Naming conventions
  • Units
  • Global variables
  • Misc. syntax
  • Algebraic syntax
  • Topology Rules
• HSPICE Hints
• Running HSPICE
  • Text interface
  • Graphical interface

General Info

The history of HSPICE includes:

• 1981 - HSPICE introduced
• 1984 - HSPICE capable of 50,000 node analysis
• 1985 - Meta-Labs established
• 1987 - Optimization added to HSPICE
• 1988 - Speed of HSPICE increased by 10-100X; 100,000 transistors
• 1989 - Mixed signal analysis integrated into HSPICE; P.C. version marketed
• 1990 - Lossy transmission line analysis incorporated into HSPICE
• 1991 - GSI added for x-windows
• 1992 - Major improvements in speed, accuracy, and convergence
• 1993 - Automatice memory allocation added
• 1995 - Improvements in speed and versatilty

What does SPICE mean?

• Sick Persons Idea of Cerebral Entertainment
• Special Program Intended to Confuse Engineers
• Society for the Prevention of Intelligence in otherwise Competent Engineers
• Simulation Program Intended to Complement Engineering
• Simulation Program with Integrated Circuit Emphasis

HSPICE Files

Suffixes:

• HSPICE Input
  • input netlist: .sp
  • design configuration: .cfg
  • initialization: hspice.ini
  Note: The italicized files those that you must have.
• HSPICE Output
  • run status: .st0
  • output listing: .lis
  • graph data, transient: .tr# (e.g. .tr0)
  • graph data, dc: .sw# (e.g. .sw2)
  • graph data, ac: .ac# (e.g. .ac1)
  • measure output: .m*# (e.g. .mt0)
  Note: The italicized files are those that you will always have.

File Descriptions:

Netlist file (.sp)

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

	title			-Implicit first line; becomes netlist file title
	.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
	sources			-stimulus
	netlist			-circuit descriptions
	.model libraries	-.lib and .inc
	.end			-terminates the simutlation

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 netlist		$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

Another example of a bjt amplifier bias by a voltage divider is given in bjtamp.sp.

Design configuration (.cfg)

Configuration files are used by HSPICE, GSI and HSPLOT to describe the available terminals and hardcopy devices. There is already a default .cfg file (meta.cfg) that already has all the printer and terminal types used at the ECE labs so it is unlikely that this file will need to be created.

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 statuts file keeps track of all that HSPICE preforms on a netlist file. Since no results are stored here, just execution steps, this file is not very useful and can be deleted without any great loss to a user. The does sometimes offer small benefit for debugging purposes as it can show which steps were not preformed by HSPICE.

A run status file from the bjt example is listed in bjtamp.st0.

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):

1. HSPICE licensing information
2. Listing of the circuit
3. Results form the analysis of the circuit (.op, .print, .plot, .measure, .ac, and .tran in order of their appearance in the netlist file)

The .lis file for the bjt ampliphier netlist above is shown in bjtamp.lis.

Graph data files (.tr#, .sw#, .ac#)

Graph data files are created by .OPTION POST command and contain the data to graphed by HSPLOT, GSI, 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 arn't very useful either as the data is hard to read and already exits in a nicely formated way in the .lis file.

An example .m*# file from the bjt ampliphier example of above is displayed in bjtamp.ma0.

Netlist Notation:

Naming conventions:

• Node and Element Identification
  • Either Names or Numbers (e.g. n1,33,in1,100)
  • Numbers: 1 to 99999999 (99 million)
  • Nodes with number followed by letter are all the same (e.g. 1a=1b)
  • 0 is ALWAYS ground
  • Capitals do not matter (e.g. node1=NODE1=Node1=nOdE1)
• Allowable Characters and Conventions (if nodes have names and not just numbers)
  • Begin with letter or /
  • Max of 16 characters (after 16 ignored)
  • May contain: +-*/:;$#.[]!<>_%
  • May not contain: (),=<space>
  • Ground may be either 0, gnd, or !gnd
• Every node must have at least 2 connections.

HSPICE units:

• R - ohm
• C - Farad
• L - Henry

• 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.
  • Assigns common node name to subcircuit nodes
  • Power supply connection of all subcirsuits often done this way
    • .GLOBAL VCC
    • Connects all nodes named VCC (all circuits have a common node)

Misc. Syntax:

• <*> - indicates a full line comment
• <$> - indicates a end of line comment
• <+> - indicates a coninuation of the previous line

Algebraic Syntax:

• sin(x)
• cos(x)
• tan(x)
• atan(x)
• exp(x)
• log(x) - this function will use the abs value of x and then apply the sign of x to the results.
• pwr(x,y) - x to power y, see also log.
• sinh(x)
• cosh(x)
• tanh(x)
• sqrt(x) - see also log
• db(x)
• log10(x) - see also log
• abs(x)
• min(x,x)
• max(x,x)

Some examples of using algebaic functions in HSPICE are:

• Parameterization (variable declaration)
  

  	.PARAM x='y+3'

• In elements
  

  	r1	1	0	r='abs(v(1)/i(m1))+10'

• In .MEASURE statements
  

  	.MEAS vmax MAX V(1)
  	.MEAS imax MAX I(q2)
  	.MEAS ivmax PARAM='vmax*imax'

Topology Rules:

• Every node must have a DC path to ground (i.e. all circuits must a have at least one ground not in series with a capacitor).
• No dangling nodes (i.e. all nodes must have at least two connections).
• No voltage loops (i.e. no voltage sources in parallel with no other elements).
• No ideal voltage source in closed inductor loop.
• No stacked current sources (i.e. no current sources in series).
• No ideal current source in closed capacitor loop.

HSPICE Hints:

1. Know what to expect from the simulation BEFORE running it!!!
2. Simulation is NO substitute for THINKING.

Other helpful hints are these:

1. It is not required to use one of HSPICE's graphing programs. One of the most common ways is to extract the graphing data from the .lis file using scripts and then use Matlab to graph the data. For a more complete discription of the process check out the graphing page.
2. It is not required to use the HSPICE graphical interface. Though the HSPICE text interface is not as pretty as the graphical interface, it is much faster and does not pull very hard on system resources. To find out how to run HSPICE using just the text interface check out Running HSPICE.
3. It is helpful to use a makefile to run HSPICE. A makefile keeps the directories clean of useless files and can automatically graph the results. Check out the Makefile that I use (Note GetTran and GetAc are scripts that remove AC and Transient analysis data from the .lis file to graph in Matlab).

Running HSPICE:

Text Interface:

1. Create the nestlist (.sp) file using any available text editor (vi, pico, emacs, nedit, etc.).
2. To run the HSPICE simulation type in
   

   	hspice <filename>.sp > <filename>.lis

3. View the results (.lis file)

Graphical Interface:

1. Make sure x-windows is running
2. Move the mouse pointer onto the empty desktop
3. Press the left most button to call up the Utilities menu
4. Select Hspice under Applications