HSPICE 98.4 Tutorial

• Introduction
• Preparation
• Editing HSPICE Input Netlist
• Starting HSPICE
• Printing and Plotting

In this tutorial, we will illustrate how to write a input netlist, the different modes available for the analysis , saving the results of analysis and using AWAVES to observe and measure various plots saved during simulation. we will illustrate all this with a simple CMOS inverter as shown in Fig.1 below.

In this figure, there are two transistors of the same dimensions, L = 1u and W = 20u and their gates are connected together at node IN.

pch is the p-channel or PMOS transistor. Its terminals, drain, gate and source are connected to nodes OUT, IN and VCC respectively.

nch is the n-channel or NMOS transistor. Its terminals, drain, gate and source are connected to nodes OUT, IN and 0 respectively.

In order to use HSPICE, modify your .profile file with

setup hspice

Don't forget to execute

.  .profile

• Use any text editor to enter the example HSPICE source code file listed below for DC Sweep and transient time analysis:

 

 
 
 
 
 

Inverter Circuit
* example circuit

.OPTIONS LIST NODE POST
.TRAN 200P 20N SWEEP TEMP -55 75 10
.PRINT TRAN V(IN) V(OUT)

M1 OUT IN VCC VCC PCH L=1U W=20U
M2 OUT IN 0 0 NCH L=1U W=20U

VCC VCC 0 5
VIN IN 0 0 PULSE .2 4.8 2N 1N 1N 5N 20N
CLOAD OUT 0 .75P               $ this is the load capacitance

.MODEL PCH PMOS
.MODEL NCH NMOS

.ALTER CLOAD OUT 0 1.5P

.END

Statements in the input netlist file can be in any order, except that the first line is a title line, and the last .ALTER submodule must appear at the end of the file before the .END statement. If there is no .END statement at the end of the input netlist file or no carriage return after the .END statement, an error message is issued.

You can place comment statements anywhere in the circuit description. The * must be in the first space on the line. The $ must be used for comments that do not begin at the first space on a line (for example, for comments that follow Hspice input on the same line). The $ must be preceded by a space or comma if it is not the first nonblank character. The $ is allowed within node or element names.

Following conventions must be followed in naming elements. The first letter for each of the elements should be as in the table below.
 

B	IBIS buffer
C	Capacitor
D	Diode
E,F,G,H	Dependent current and voltage sources
I	Current source
J	JFET or MESFET
K	Mutual inductor
L	Inductor
M	MOSFET
Q	BJT
R	Resistor
T,U,W	Transmission line

M1 is the name given to the pch transitor shown in the Fig. 1. This is followed by the node numbers of the drain, gate, source and substrate of the transistor in this specific order. These node numbers are exactly the same as shown in Fig. 1. Then PCH indicates that transistor M1 is of p-channel model defined on later in the files. In a similar fashion, the drain, gate, and source of the nch, M2, are connected respectively to OUT , IN and 0. The latest node is the ground. NCH refers to the model of this transistor. The other entries give the width and length of the channel. The next line describes how the load capacitance, C3, is connected accross the output, node OUT and ground, node 0.

Next the voltage sources are defined. VCC VCC 0 5, tell us that a DC source of 5V is applied accross node VCC and ground. Also, a voltage, VIN is applied at the gates of the transistors, node IN. The value of this source is then specified on the next line. VIN takes a pulse input as specified. the lines starting with .MODEL define the transistor models, PCH and NCH.

.ALTER statement is used to rerun a simulation using different parameters and data, here value of load capacitance is changed from initial value of 0.75 pico farad to 1.5 pico farad.
.TRAN statement causes Hspice to perform a multipoint transient analysis for 20 ns for temperatures ranging from -50¯C to 75¯C in steps of 10¯C.
 

• Save this example SPICE source code as "inverter.sp"
click here to go back to Index

Starting HSPICE

Invoke Hspice with a UNIX command:

$ hspice example.sp > example.lis &

Various output files that may be generated are listed below:
 

Output File Type	Extension
Output listing	.lis, or user-specified
Transient analysis results	.tr# *
Transient analysis measurement results	.mt#
DC analysis results	.sw# *
DC analysis measurement results	.ms#
AC analysis results	.ac# *
AC analysis measurement results	.ma#
Hardcopy graph data (from meta.cfg PRTDEFAULT)	.gr# **
Digital output	.a2d
FFT analysis graph data	. ft#***
Subcircuit cross-listing	. pa#
Output status	. st#
Operating point node voltages (initial conditions)	. ic

# is either a sweep number or a hardcopy file number.
* Only created if a .POST statement is used to generate graphical data.
** Requires a .GRAPH statement or a pointer to a file exists in the meta.cfg file.
     This file is not generated by the PC version of Star-Hspice.
*** Only created if a .FFT statement is used.

Type,

$ hspice inverter.sp > inverter.lis &

to start hspice and load the example you have edited.

You will see following message on the screen

>info:         ***** hspice job concluded
>info:         ***** hspice job concluded
user        0.6
sys         0.4

Following files are generated as a result:
 

inverter.lis	Output Listing
inverter.ic	Operating point node voltages (initial conditions)
inverter.st0	Output Status
inverter.tr0	Transient analysis results for the 1st CLOAD value
inverter.tr1	Transient analysis results for the 2nd CLOAD value

click here to back to Index:

Printing and Ploting

Using Output Statements

Hspice output statements are contained in the input netlist file and include .PRINT, .PLOT, .GRAPH, .PROBE, and .MEASURE. Each statement specifies the output variables and type of simulation  result to be displayed. For example, .DC, .AC, or .TRAN. With the use of .OPTION POST, all output variables referenced in .PRINT, .PLOT, .GRAPH, .PROBE, and .MEASURE statements are put into the interface files for AvanWaves. AvanWaves allows high resolution, post simulation, and interactive display of waveforms.
 
 

Output Statement	Brief Description of Use
.PRINT	Prints numeric analysis results in the output listing file (and post-processor data if .OPTION POST is used).
.PLOT	Generates low-resolution (ASCII) plots in the output listing file(and post-processor data if .OPTION POST is used).
.GRAPH	Generates high-resolution plots for specific printing devices (HP LaserJet for example) or in PostScript format, intended for hard-copy outputs without a using a post-processor.
.PROBE	Outputs data to post-processor output files but not to the output listing (used with .OPTION PROBE to limit output).
.MEASURE	Prints to output listing file the results of specific user-defined analyses (and post-processor data if .OPTION POST is used).

To observe the results of the simulation, invoke awaves by typing

$ awaves&

open the design inverter.sp . We can display input and output voltages for CLOAD value of 0.75pf as well as 1.5pf simultaneously or one at a time. Output voltage is plotted for the range of temperature as specified in the inverter.sp netlist.

We can select the curve to be displayed in the result browser window.
 
 




 

Fig. 2 Result Browser

The actual waveforms for V(IN) and V(OUT) for CLOAD = 1.5pf are displayed as below
 
 





Fig.3 V(IN) and V(OUT) with CLOAD = 1.5pf

To print the plot click on the Printbutton or select Print from the Tools.

We can either save the plot as a postscript file or print it rightaway.
 
 





Fig.4 Print Menu





---

For any further question or problems you can refer to the online pdf documentation available at /opt/hspice-98.4/docs

---

click here to back to Index:

---

Click here to go to 'VLSI Design Flow Using Mentor-Graphics Tools'

Click here to go to the main Helpme menu.