|
Nspice is the encapsulated spice simulator that
performs a spice(1ICD) analysis for a circuit cell that is
present in the database, using a commandfile with spice
and/or sls(1ICD) commands. Nspice consists of a unix
shell-script that extracts a circuit cell from the database
using xsls(1ICD), converts a commandfile with spice
and/or sls commands to a spice commandfile using
nspice_pp, runs spice, and finally executes
nspice_bs to backsubstitute node numbers in the
output file by their corresponding names as specified in the
database. The output of nspice is found in a file
called cell.ana.
nspice_pp: The program nspice_pp converts,
for a particular cell (first program argument), a
commandfile with spice and/or sls commands (second program
argument) to a spice commandfile. In the inputfile nodes may
be referred to by their names as specified in the database.
The output of the program is sent to stdout. The
conversion is executed by using information from a spice
network description that is present in the file
cell.spc. This file is typically extracted from the
database using xsls with the options -Shlmbf. This
will generate a file cell.spc with a full
(hierarchical) description of the cell, including the
appropriate transistor models, terminals for n-bulk and/or
p-bulk connections, and a name translation table that
translates node numbers into node names as used in the
database. To reduce the number of nodes in the spice network
description the use of the options -xy [ -z name ] is
further recommended (see manual page of xsls ).
All sls commands that are allowed with the sls
simulator (see "sls: switch-level simulator
user's manual") may be used in the commandfile of
nspice_pp. However the ones that are translated into
spice commands are the following: The set commands in the
commandfile are translated into piecewise linear voltage
sources that are connected to the relevant input nodes of
the network. Sls plot commands are translated into
".print tran node1 node2 ..." cards. If
option level=3 is specified, a transient analysis card will
be placed in the outputfile that specifies a simulation from
t=0 till t=t_end, where t_end is given by simperiod x
sigunit or otherwise - if simperiod is not specified - by
the time of the last input signal transition. The value of
tstep in the .tran card should explicitly be defined in the
commandfile (see below).
The other information that is allowed in the commandfile
should be specified in the following way:
*%
... translation information ...
*%
... direct spice commands ...
*%
The separators '*%' should be placed at the
beginning of each line. The first part consists of
translation information that is used to translate sls
commands (if any) into spice commands. It may consist of
zero or more of the following lines
tstep <real>
tstart <real>
uic
trise <real>
tfall <real>
vhigh <real>
vlow <real>
The field <real> denotes a specification of a real
value. It may optionally have a scale factor 'G'
(1e9), 'M' (1e6), 'k' (1e3),
'm' (1e-3), 'u' (1e-6),
'n' (1e-9), 'p' (1e-12) or
'f' (1e-15). The variable tstep specifies
the value of tstep as used for transient analysis. This
value should be specified when option level=3 is used with
the sls commands (see above). The variable tstart
optionally specifies the start time for the transient
analysis card. If the keyword uic is used, this
keyword will be added to the .tran card. The variables
trise and tfall respectively specify the rise
and fall time of the input signals (default trise = tfall =
tstep). The variables vhigh and vlow
respectively specify the voltages that correspond to the
high state and the low state of the input signals (default
vhigh = 5 and vlow = 0). For the x state a voltage of (vhigh
+ vlow) / 2 is used.
In the second part of the spice information, direct spice
commands may be specified. These commands are directly
copied to the output, however with node names that are
specified between quotes translated to their corresponding
node numbers. E.g. .ic v("out")=5v might be
translated into .ic v(12)=5v. If no sls commands are used,
this part of the commandfile - beside the information that
is extracted with xsls - will contain all the
information that is necessary for the spice simulation.
An example of a commandfile with only spice commands is
given below:
*%
*%
vphi1 "phi1" 0 pulse (5v 0v 29.4ns 0.6ns 0.6ns 29.4ns 60ns)
vphi2 "phi2" 0 pulse (0v 5v 29.4ns 0.6ns 0.6ns 29.4ns 60ns)
vvdd "vdd" 0 5v
vin "in" 0 pulse (5v 0v 29.4ns 0.6ns)
.tran 0.2n 120n
.print tran v("phi1") v("phi2") v("1") v("2") v("3")
.print tran v("4") v("in") v("out") v("out_inv")
.options nomod
.options limpts=601
.options cptime=100
.ic v("3")=0 v("out")=5
*%
An example of a commandfile with mixed sls and spice
commands is as follows:
set phi1 = (h*30 l*30)*~
set phi2 = (l*30 h*30)*~
set vdd = h
set vss = l
set in = h*30 l
option level = 3
option simperiod = 120
option sigunit = 1n
option outacc = 10p
plot phi1 phi2 1 2 3 4 in out out_inv
/*
*%
tstep 0.2n
trise 0.6n
tfall 0.6n
*%
.options nomod
.options limpts=601
.options cptime=100
.ic v("3")=0 v("out")=5
*%
*/
(Note that the spice information is placed between sls
comment signs ("/*" and "*/") so as to
allow to use the same inputfile for an sls simulation.)
nspice_bs: The program nspice_bs
backsubstitutes node numbers by node names in a spice output
file for a cell (specified as an argument). This is done
according to a name translation table that should be present
in a file called cell.spc. The name of the spice
output must be cell.ana. Nspice_bs will only
backsubstitute node numbers that are in the header of a
transient analysis table.
The nspice unix-shell script has the following form:
# xsls: always use options -Shlmbf;
# the use of options -xy [ -z name ] is recommended
xsls -Shlmbf -xy $1
nspice_pp $1 $2 >> $1.spc
spice $1.spc > $1.ana
if nspice_bs $1
then
exit 0
else
exit 1
fi
# eof
|
