This is ngspice.info, produced by makeinfo version 4.8 from
ngspice.texi.

INFO-DIR-SECTION Utilities
START-INFO-DIR-ENTRY
* NGSPICE: (ngspice).              NGSPICE User Manual
END-INFO-DIR-ENTRY

   Copyright 1996 The Regents of the University of California.

     Permission to use, copy, modify, and distribute this software and
     its documentation for educational, research and non-profit
     purposes, without fee, and without a written agreement is hereby
     granted, provided that the above copyright notice, this paragraph
     and the following three paragraphs appear in all copies.

     This software program and documentation are copyrighted by The
     Regents of the University of California. The software program and
     documentation are supplied "as is", without any accompanying
     services from The Regents. The Regents does not warrant that the
     operation of the program will be uninterrupted or error-free. The
     end-user understands that the program was developed for research
     purposes and is advised not to rely exclusively on the program for
     any reason.

     IN NO EVENT SHALL THE UNIVERSITY OF CALIFORNIA BE LIABLE TO ANY
     PARTY FOR DIRECT, INDIRECT, SPECIAL, INCIDENTAL, OR CONSEQUENTIAL
     DAMAGES, INCLUDING LOST PROFITS, ARISING OUT OF THE USE OF THIS
     SOFTWARE AND ITS DOCUMENTATION, EVEN IF THE UNIVERSITY OF
     CALIFORNIA HAS BEEN ADVISED OF THE POSSIBILITY OF SUCH DAMAGE. THE
     UNIVERSITY OF CALIFORNIA SPECIFICALLY DISCLAIMS ANY WARRANTIES,
     INCLUDING, BUT NOT LIMITED TO, THE IMPLIED WARRANTIES OF
     MERCHANTABILITY AND FITNESS FOR A PARTICULAR PURPOSE. THE SOFTWARE
     PROVIDED HEREUNDER IS ON AN "AS IS" BASIS, AND THE UNIVERSITY OF
     CALIFORNIA HAS NO OBLIGATIONS TO PROVIDE MAINTENANCE, SUPPORT,
     UPDATES, ENHANCEMENTS, OR MODIFICATIONS.


File: ngspice.info,  Node: Top,  Next: Preface,  Prev: (dir),  Up: (dir)

NGSpice User Manual
*******************

This manual describes the mixed level simulator NGspice and applies to
the version called Rework 17.

   Copyright 1996 The Regents of the University of California.

     Permission to use, copy, modify, and distribute this software and
     its documentation for educational, research and non-profit
     purposes, without fee, and without a written agreement is hereby
     granted, provided that the above copyright notice, this paragraph
     and the following three paragraphs appear in all copies.

     This software program and documentation are copyrighted by The
     Regents of the University of California. The software program and
     documentation are supplied "as is", without any accompanying
     services from The Regents. The Regents does not warrant that the
     operation of the program will be uninterrupted or error-free. The
     end-user understands that the program was developed for research
     purposes and is advised not to rely exclusively on the program for
     any reason.

     IN NO EVENT SHALL THE UNIVERSITY OF CALIFORNIA BE LIABLE TO ANY
     PARTY FOR DIRECT, INDIRECT, SPECIAL, INCIDENTAL, OR CONSEQUENTIAL
     DAMAGES, INCLUDING LOST PROFITS, ARISING OUT OF THE USE OF THIS
     SOFTWARE AND ITS DOCUMENTATION, EVEN IF THE UNIVERSITY OF
     CALIFORNIA HAS BEEN ADVISED OF THE POSSIBILITY OF SUCH DAMAGE. THE
     UNIVERSITY OF CALIFORNIA SPECIFICALLY DISCLAIMS ANY WARRANTIES,
     INCLUDING, BUT NOT LIMITED TO, THE IMPLIED WARRANTIES OF
     MERCHANTABILITY AND FITNESS FOR A PARTICULAR PURPOSE. THE SOFTWARE
     PROVIDED HEREUNDER IS ON AN "AS IS" BASIS, AND THE UNIVERSITY OF
     CALIFORNIA HAS NO OBLIGATIONS TO PROVIDE MAINTENANCE, SUPPORT,
     UPDATES, ENHANCEMENTS, OR MODIFICATIONS.

* Menu:

* Preface::                     Some words about this manual.
* Acknowledgements::            Almost all the people who contributed
                                  to NGSPICE development.
* Release Notes::               Release notes for the NGSPICE simulator
* Introduction::                Description of NGSPICE. Try to answer
                                  the question: What NGSPICE is ?
* NGSPICE Compilation::         How to compile NGSPICE.
* Supported Analyses::          Describes supported analyses and introduces
                                  some convergence issues.
* Circuit Description::         How to input a circuit to the simulator.
* Circuit Elements and Models:: Description and use of the devices models
                                  built into NGSPICE.
* Analyses and Output Control:: How to run analyses and check the results.
* Interactive Interpreter::     The commands recognized by the NGSPICE
                                  interactive frontend.
* Bibliography::                A small bibliography.
* Example Circuits::            Some examples.
* Model and Device Parameters:: Equations that makes the models and parameters.


File: ngspice.info,  Node: Preface,  Next: Acknowledgements,  Prev: Top,  Up: Top

1 Preface
*********

The NGSPICE user's manual is based on the text file included in the
Spice3f source package. The original text has been converted to TeXInfo
format by Emmanuel Rouat and Arno W. Peters.

   The original text has been modified and extended to reflect the
changes between plain Spice3f5 and NGSPICE. Some of the "changes" comes
from the HTML documentation Charles D.H. Williams has written and
published on his web site.

   This manual covers the double role of being an introductory text for
the novice user who wants to learn how to use spice (and thus NGSPICE),
and a reference text for the expert who wants to identify the
differences between the original spice3f code (sometimes referred as
the Berkeley's Spice) and the NGSPICE code.

   Since NGSPICE is an Open Source software, one chapter describing
program compilation and compilation options have been added to the
original text. Since its birth, spice3f had many compilation switches
that enabled/disabled some features considered experimental or
troublesome. In a "perfect world", most of these switches would be
implemented as runtime options, thus allowing users to
activate/deactivate the features they want without recompiling the
source. Anyway time is never sufficient to implement all the features
and, in the end, this is not a "perfect world".

   Trying to keep a record of the "long" history of this piece of
software, an entire chapter has been dedicated to the description of
the patches publicly made available in the past years through USENET
newsgroups.

   As always, errors, omissions and unreadable phrases are only my
fault.
                                         Paolo Nenzi <p.nenzi@ieee.org>
                                                  Roma, March 24th 2001

     Indeed. At the end of the day, this is engineering, and one learns
     to live within the limitations of the tools.
          Kevin Aylward <kevin@anasoft.co.uk> , Warden of the Kings Ale


File: ngspice.info,  Node: Acknowledgements,  Next: Release Notes,  Prev: Preface,  Up: Top

2 Acknowledgements
******************

Spice was originally written at The University of California at
Berkeley (USA).  Since then, there have been many people working on the
software, most of them releasing patches to the original code through
the Internet.

   The following people have contributed in some way:


Vera Albrecht <albrecht@danalyse.de>,
Cecil Aswell <aswell@netcom.com>,
Steven Borley <steven.borley@virgin.net>,
Stuart Brorson <sdb@cloud9.net>,
Giles C. Billingsley,
Mansun Chan,
Wayne A. Christopher,
Al Davis <aldavis@ieee.org>,
Glao S. Dezai <dezai@hotbot.com>,
Jon Engelbert <jon@beigebag.com>,
Daniele Foci <d.foci@ieee.ing.uniroma1.it>,
Noah Friedman <friedman@prep.ai.mit.edu>,
Alan Gillespie <Alan.Gillespie@analog.com>,
David A. Gates,
JianHui Huang,
Jeffrey M. Hsu,
S. Hwang,
Chris Inbody <cinbody@cowtown.net>,
Gordon M. Jacobs,
Min-Chie Jeng,
Stefan Jones <stefan.jones@multigig.com>,
Beorn Johnson <beorn@eecs.berkeley.edu>,
Kenneth H. Keller,
Mathew Lew,
Robert Lindsell <robertl@research.canon.com.au>,
Weidong Liu,
Kartikeya Mayaram,
Richard D. McRoberts <rdm@csn.net>,
Manfred Metzger <ManfredMetzger@gmx.de>,
Paolo Nenzi <pnenzi@ieee.org>,
Gary W. Ng,
Wolfgang Muees,
Hong June Park,
Arno Peters <A.W.Peters@ieee.org>,
Serban-Mihai Popescu <serbanp@ix.netcom.com>,
Georg Post <georg.post@wanadoo.fr>,
Thomas L. Quarles,
Emmanuel Rouat <emmanuel.rouat@wanadoo.fr>,
Jean-Marc Routure <routoure@greyc.ismra.fr>,
Jaijeet S. Roychowdhury,
Takayasu Sakurai,
AMAKAWA Shuhei <sa264@cam.ac.uk>,
Kanwar Jit Singh,
Hitoshi Tanaka <HDA01055@nifty.com>,
Steve Tell <tell@cs.unc.edu>,
Andrew Tuckey <Tuckey@ieee.org>,
Charles D.H. Williams <C.D.H.Williams@exeter.ac.uk>,
Holger Vogt <holger.vogt@uni-duisburg.de>,
Dietmar Warning <warning@danalyse.de>,
Michael Widlok <widlok@uci.agh.edu.pl>,
Antony Wilson <wilsona@earthlink.net>,
and many others...

   If someone helped in the development and has not been inserted in
this list then this omission was unintentional. If you feel you should
be on this list then please write to
<ngspice-devel@lists.sourceforge.net>. Do not be shy, we would like to
make a list as complete as possible.


File: ngspice.info,  Node: Release Notes,  Next: Introduction,  Prev: Acknowledgements,  Up: Top

3 Release Notes
***************

NGSPICE REWORK-14 RELEASE (released on December 10th, 2001):

     This release fixes most of the bugs that appeared in rework-13.

     Some leaks in the frontend have been closed.

     GNU Autoconf interface cleaned (better support for getopt).

     Better error reporting (thanks to Charles Williams "CDHW").

     Added mesa tests (macspice3f4).

     Added support for ekv model (not source code).

     The Rawfile format changed again removing "Probe" compatibility code.

NGSPICE REWORK-13 RELEASE (released on November 5th, 2000):

     This is a major release in terms of fixes and enhancements.

     A garbage collector support has been added. If the configuration
     script detects that you have installed GC (Bohem-Weiser conservative
     garbage collector), it will use it.

     Some memory leaks have been fixed too.

     Enhancements to the code comes from Alan's (Gillespie) contribute
     code, a description of improvements follows (extracted form
     Alan's mail):

     * Output File Format Changes -

     Rawfile format changed to PSPICE Probe format (Usable with Demo
     version of Microsim's Probe). (NOTE: Do not rely on this, we may
     revert to the old format in the next release).

     Text mode .OP results even though "rawfile" written.

     Internal device nodes are not saved to "rawfile" (reduces file
     size). Optionally, these internal nodes can be replaced by device
     currents and saved.

     * DC Convergence Enhancements -

     "Source-Stepping" algorithm modified with a "Dynamic" step size.
     After each successful step, the node voltages are saved, the
     source-factor is increased by the step-factor, and the step-factor
     is increased (for the next step). If the step fails, i.e. the
     circuit does not converge, the source-factor is set to the value
     from the previous successful step, the previously stored node
     voltages are restored, the step-factor is reduced, the source factor
     is increased by this smaller step-factor, and convergence is
     attempted again.

     Same thing done for "Gmin-stepping" algorithm.

     "Gshunt" option added. This sets the "diagGmin" variable used
     in the gmin-stepping algorithm to a non-zero value for the final
     solution. (Normally this is set to zero for the final solution).
     This helps for circuits with floating nodes (and for some others too).

     The Gmin implementation across the substrate diodes of MOS1, MOS2,
     MOS3, MOS6 and BSIM3 devices, and across BJT base-emitter and
     base-collector diodes, was incorrect. Correcting this dramatically
     improved DC convergence. (I think this also effects BSIM1 and 2 but
     I haven't fixed them yet! ).

     The gm, gmb and gds calculations in the MOS3 model were all wrong.
     The device equations were fixed, leading to much improved convergence.

     The Vcrit value used for diode voltage limiting was calculated without
     taking into account the device area (and in some cases without using
     the temperature corrected saturation current). This could cause floating
     point overflows, especially in device models designed to be scaled by a
     small area, e.g. 2u by 2u diodes (area=4e-12). This is now fixed for
     Diode, BJT, MOS1, MOS2, and MOS3 models.

     The diode voltage limiting was modified to add negative voltage
     limiting. Negative diode voltages are now limited to 3*Vdp-10, where
     Vdp is the voltage from the previous iteration. If Vdp is positive,
     then the voltage is limited to -10V. This prevents some more floating
     point overflows. (Actually, I'm still playing with the best values for
     this).

     The Spice3 "fix" for the MOS3 gds discontinuity between the linear and
     saturated regions only works if the VMAX parameter is non-zero. A
     "tweak" has been added for the VMAX=0 case.

     * Transient Convergence Enhancements -

     Temperature correction of various diode capacitances was implemented
     slightly incorrectly, leading to capacitance discontinuities in
     simulations at temperatures other than nominal. This affected the
     Diode and MOS3 models.

     A mistake in the implementation of the MOS3 source-bulk capacitance
     model resulted in a charge storage discontinuity. This has been fixed.

     The level 2 MOSFET model seems to calculate Von and Vth values for the
     threshold and subthreshold values respectively, but then uses Vbin to
     calculate the Vdsat voltage used to find the drain current. However, a
     jump statement uses Von to decide that the device is in the "cutoff"
     region, which means that when this jump allows the drain current to be
     calculated, Vdsat can already be well above zero. This leads to a
     discontinuity of drain current with respect to gate voltage. The code
     is now modified to use Vbin for the jump decision. It looks like the
     code should actually use Vth as the threshold voltage, but since
     PSPICE and HSPICE both follow the original Berkeley code, this was
     left alone.

     * New Model Parameters -

     A PSPICE/HSPICE-like "M" device parameter (i.e. M devices in parallel)
     was added to the MOS1,2,3 and BSIM3 mosfet models.

     * Input Read-in and Checking -

     Numbers beginning with a "+" sign got the input routine confused.
     Fixed now.

     Attempts to nodeset (or .IC) non-existent nodes are flagged with
     a warning.

     PWL statements on Voltage or Current sources are now checked for
     "non-increasing" time-points at the start of the simulation.
     Previously each time-point was checked as it was reached during
     the simulation, which could be very annoying if you made a mistake
     which caused the simulation to fail after hours of run-time.

     A check which was performed at the end of each sub-circuit
     expansion was moved to the top level. This check makes sure that
     all sub-circuits have been defined, but in its original position,
     it meant that if a sub-circuit included ANY .MODEL statements at all,
     then ALL the models called in that sub-circuit must also be defined
     within that sub-circuit. Now SPICE behaves as expected, i.e. a
     subcircuit may define its own models, but may also use models defined
     at any level above.

     * Miscellaneous Fixes/Enhancements -

     MOS devices reported only half of the Meyer capacitances, and did
     not include overlap capacitances, when reporting to the .OP printout,
     or when storing device capacitances to the "rawfile".

     The ideal switch devices had no time-step control to stop their
     controlling voltages/currents overshooting the switching thresholds.
     The time-step control has been modified to use the last two time
     points to estimate if the next one will move the controlling
     voltage/current past a switching threshold. If this looks likely,
     then the time-step is reduced.

     The "rawfile" writing routines have been modified to print the
     "reference value" to the console during the simulation. This lets
     the user see exactly how far and how fast the simulation is proceeding.

     .OP printout tidied up a lot to make the printout clearer.

     Analysis order changed to fix a "feature" where, if you ask for a
     .OP and a .TRAN in the same simulation, the node voltages printed out
     correspond to the .OP, but the device data was from the last timepoint
     of the .TRAN.

NGSPICE REWORK-12 RELEASE (released on August 26th, 2000):

     Arno did a great work this summer!
     This release consists of his work. The pole-zero analysis has been
     corrected. The error was introduced in an attempt to eliminate compiler
     warnings.

     The source has been reworked and info file have been updated.
     As you may see, a new dir called "spicelib" has been created, another
     step toward the separation of the simulator from the frontend.

NGSPICE REWORK-11 RELEASE (released on May 28th, 2000):

     The code has been cleaned, the resistance code for ac parameter
     has been modified to conform to Spice3 parameter parsing.

     A new step function has been introduced (u2).

     Updated documentation to reflect changes.

NGSPICE REWORK-10 RELEASE (released on April 5th, 2000):

     All devices are compiled as shared libraries (ld.so).

     There is an initial support for the BSIM4 model. This release
     is to be considered as baseline for the project.

     There are still some harmless bugs in the resistor code.

   Release notes for older NGSPICE release are not available. For
historical purpose only the following release notes, pertaining to the
original Spice3 code have been included into this manual. They have
been copied from "SPICE 3 Version 3f5 User's Manual":

   Spice3f is the six major release of Spice3. This release incorporates
new features not available in Spice 3c or 3d, as well as several
performance improvements. All of the feature described here are believed
to be fully functional. The development of SPICE is ongoing at Berkeley,
and therefore not all of the intended capabilities have been implemented
in full yet.

BUGS IN 3F2 FIXED IN 3F3:

     Ascii (printer) plots in spice3f2 did not print bode plots vs log of the
     frequency by default, as in spice2.

     You had to explicitly request the x-axis to be log; either "`plot
     vdb(2) xlog'" (best) or "`plot vdb(2) vs log10(frequency)'" will
     do. Now, simply "`plot vdb(2)'" will work.

     The on-line documentation has been brought up to date by converting this
     manual into a format readable on-line.

     Significant problems with AC sensitivities in 3f2 only have been fixed.

     Multiple analyses and plots in spice2 emulation mode under 3f2 and
     earlier generated misleading error messages. This no longer happens
     in 3f3.

NEW FEATURES AND BUG FIXES INCORPORATED IN SPICE3F (the current release
of Spice3):

     Sensitivity analysis
     Added a parameter for fitting JFET models (parameter "`B'").

     Fixed a discontinuity problem in MOS level 3 (related to the
     "`kappa'" parameter). Working "`alter'" command.

     Improved "`show'" and "`showmod'" commands for operating points
     summary tables (like Spice2).

     Working "`trace'" command.

     Interactive "`set'" variable values now the same as
     "`.options'" settings.

     Improved plotting, including implicitly transforming data for smith
     plots.

     Added function "`deriv()'" (derivative) to the front-end.

     Corrected an error affecting the specified initial conditions for
     some circuits.

     Miscellaneous bug fixes in the front-end.

NEW FEATURE AND BUGS FIXES INCORPORATED IN SPICE3E (the _previous_
release of Spice3):

     Lossy Transmission lines.

     Proper calculation of sheet resistance in the MOS models.

     A new command ("`where'") to aid in debugging troublesome
     circuits.

     Smith-chart plots working (see the "`plot'" command).

     Arbitrary sources in subcircuits handled correctly.

     Arbitrary source reciprocal calculations and DC biasing fixed.

     Minor bug-fixes to the Pole-Zero analysis.

     Miscellaneous bug fixes in the front end.

SOME COMMON PROBLEMS REMAINING IN SPICE3F (note that this list is not
complete):

     Models defined within subcircuits are not always handled correctly.
     If you have trouble, move the model definition outside of "`.subckt'"
     and "`.ends'" lines.

     Batch run data is not compacted if a "rawspice" data file is generated,
     resulting in excessively large output files for some difficult inputs.

     Sufficient detail is sometimes not preserved in transient analysis.
     Providing a small value for the "`TMAX'" parameter (the fourth
     argument) in the transient run command will solve this problem.

     Convergence problems can sometimes be worked around by relaxing the
     transient "`TMAX'" parameter.

     The substrate node of the bipolar transistor (BJT) is modelled
     incorrectly (this may actually be due to inherent numerical problems
     with the model). Do not use substrate node; use a semiconductor
     capacitor to model substrate effects.

     Charge is not conserved in MOS devices based on the Meyer model.

     Transient simulation of strictly resistive circuits (typical for
     first runs or tests) allow a time step the is too large (e.g. a
     sinusoidal source driving a resistor). There is no integration
     error to restrict the time step. Use the "`TMAX'" parameter or
     include reactive elements.

     Deep nesting of subcircuits may exceed internal static buffers.

     The PZ analysis can not be interrupted; the sensitivity analysis
     can not be continued (the interactive "`resume'" command) once
     interrupted.

     There are many other small bugs, particularly in the front end.

3.1 Reporting a bug
===================

Berkeley does not provide support anymore for Spice3, if you need some
kind of help you can


File: ngspice.info,  Node: Introduction,  Next: NGSPICE Compilation,  Prev: Release Notes,  Up: Top

4 Introduction
**************

NGSPICE is a general-purpose circuit simulation program for nonlinear
dc, nonlinear transient, and linear ac analyses.  Circuits may contain
resistors, capacitors, inductors, mutual inductors, independent voltage
and current sources, four types of dependent sources, lossless and
lossy transmission lines (two separate implementations), switches,
uniform distributed RC lines, and the five most common semiconductor
devices: diodes, BJTs, JFETs, MESFETs, and MOSFETs.

   NGSPICE is a continuation of Spice3f5, the last Berkeley's release of
Spice3 simulator family.  NGSPICE is being developed to include new
features to existing Spice3f5 and to fix its bugs. Improving a circuit
simulator is a very hard task and, while some improvements have been
ported, most of the job has been done on bug fixing and code
refactoring.

   NGSPICE has built-in models for the semiconductor devices, and the
user need specify only the pertinent model parameter values.

   There are two models for BJT both based on the integral-charge model
of Gummel and Poon; however, if the Gummel-Poon parameters are not
specified, the model reduces to the simpler Ebers-Moll model. In either
case and in either models, charge storage effects, ohmic resistances,
and a current-dependent output conductance may be included. The second
BJT model BJT2 adds dc current computation in the substrate diode _but
is not fully implemented as of ngspice-rework-15_. The semiconductor
diode model can be used for either junction diodes or Schottky barrier
diodes.  There are two models for JFET: the first (JFET) is based on
the model of Shichman and Hodges, the second (JFET2) is based on the
Parker-Skellern model.  All the original six MOSFET models are
implemented: MOS1 is described by a square-law I-V characteristic, MOS2
[1] is an analytical model, while MOS3 [1] is a semi-empirical model;
MOS6 [2] is a simple analytic model accurate in the shortchannel
region; MOS4 [3, 4] and MOS5 [5] are the BSIM (Berkeley Short-channel
IGFET Model) and BSIM2.  MOS2, MOS3, and MOS4 include second-order
effects such as channel-length modulation, subthreshold conduction,
scattering-limited velocity saturation, small-size effects, and charge
controlled capacitances. Other MOS model have been implemented, like
the new BSIM3 and BSIM4 models, the SOI models from the BSIMSOI family
and the STAG one. There is partial support for a couple of HFET models
and one model for MESA devices.

   Since the rework-15 release, NGSPICE includes CIDER, a mixed-level
circuit and device simulator that provides a direct link between
technology parameters and circuit performance.

   A mixed-level circuit and device simulator can provide greater
simulation accuracy than a stand-alone circuit or device  simulator by
numerically modelling  the critical devices in a circuit.  Compact
models can be used for noncritical devices.

   CIDER couples Spice (version3) to an internal C-based device
simulator, DSIM. Spice3 provides circuit analyses, compact models for
semiconductor devices, and an interactive user interface. DSIM provides
accurate, one- and two-dimensional numerical device models based on the
solution of Poisson's equation, and the electron and hole
current-continuity equations.  DSIM incorporates many of the same basic
physical models found in the Stanford two-dimensional device simulator
PISCES. Input to CIDER consists of a SPICE-like description of the
circuit and its compact models, and PISCES-like descriptions of the
structures of numerically modeled devices.  As a result, CIDER should
seem familiar to designers already accustomed to these two tools.

   CIDER is based on the mixed-level circuit and device simulator
CODECS, and is a replacement for this program. The basic algorithms of
the two programs are the same.  Some of the differences between CIDER
and CODECS are described below. The CIDER input format has greater
flexibility and allows increased access to physical model parameters.
New physical models have been added to allow simulation of
state-of-the-art devices. These include transverse field mobility
degradation important in scaled-down MOSFETs and a polysilicon model
for poly-emitter bipolar  transistors. Temperature dependence has been
included over the range from -50C to 150C.  The numerical models can be
used to simulate all the basic types of semiconductor devices:
resistors, MOS capacitors, diodes, BJTs, JFETs and MOSFETs. BJTs and
JFETs can be modelled with or without a substrate contact.  Support has
been added for the management of device internal states.
Post-processing of device states can be performed using  the NUTMEG
user interface of Spice3.  Previously computed states can be loaded
into the program to provide accurate initial guesses for subsequent
analyses. Finally, numerous small bugs have been discovered and fixed,
and the program has been ported to a wider variety of computing
platforms.


File: ngspice.info,  Node: NGSPICE Compilation,  Next: Supported Analyses,  Prev: Introduction,  Up: Top

5 NGSPICE Compilation
*********************

* Menu:

* Extracting the archive::
* Configuring NGSPICE::
* Compiling NGSPICE::
* Supported systems::
* Platform specific issues::

   NGSPICE is an Open Source project (and software), this means that
its source code is available to the end user. Well, to be honest, the
source code is the only thing available to the user. This chapter
briefly describes how to deal with this rather complex package.


File: ngspice.info,  Node: Extracting the archive,  Next: Configuring NGSPICE,  Prev: NGSPICE Compilation,  Up: NGSPICE Compilation

5.1 Extracting the archive
==========================

NGSPICE is released as "gzipped tarball". The source tree is archived
with the `tar' command and the result compressed with `gzip'. Since the
development of the NGSPICE is carried on UNIX (mainly), all the files
have the "line feed" character as newline character and this may cause
problems when working in non UNIX environments (like DOS). If you are
going to extract NGSPICE on system that use different newline
character, you will have to convert the files with some utility.

   To extract the NGSPICE archive you need the `tar' archiver and
`gzip' compression utility:

     pnenzi@janus:~$ gzip -d ngspice-rework-15.tar.gz
     pnenzi@janus:~$ tar -xvf ngspice-rework-15.tar

   Once extracted, you  have to enter the source tree (just `cd' into
the top level directory).


File: ngspice.info,  Node: Configuring NGSPICE,  Next: Compiling NGSPICE,  Prev: Extracting the archive,  Up: NGSPICE Compilation

5.2 Configuring NGSPICE
=======================

Now that you have extracted all the files, you need to give values to
compile time variables and set the correct paths for libraries and
include file. If you have compiled other programs released in source
form, you have probably already faced the _GNU Autoconf_ system. If you
already know what Autoconf is and how it works, you can safely skip the
next paragraph.

   GNU Autoconf is a package that automates the task of configuring
source code packages. Configuring a source code package means assigning
desired values to compile-time variables, something known as
"customization", and look at functions, libraries available on the host
system to produce the makefiles needed for compilation. As said, this
is a very brief introduction to the Autoconf package, if you want to
know more, look at its documentation.

   NGSPICE uses _GNU Autoconf_ configuration tool. To configure the
package type: `./configure --help' on the command prompt. The list of
available options will be shown. The list comprises "standard" options
(the one every Autoconf package has) and options specific to the NGSPICE
package. This chapter deals with the latter only, sending back the
reader to the GNU Autoconf documentation for the former.

   The options specific to NGSPICE are:

   * `--enable-numaparam': Preliminary support for parameters expansion
           in netlists. Numparam is a library that attach itself to a
     single point        in NGSPICE code and comes with its own
     documentation. Before using this        library you should look at
     library's documentation in `src/frontend/numaparam'
     directory.

   * `--enable-ftedebug': This switch enables the code for debugging
        the NGSPICE frontend. Developers who wish to mess with the
     frontend        should enable it (and set to `TRUE' the "debug"
     option). The        casual user has no gain in enabling this
     option.

   * `--enable-ansi': This switch forces `-ansi' option of the
     for compilation. This is interesting only to developers cleaning
     the        NGSPICE code. Nore real use for the user.

   * `--enable-debug': Add `-g' option for compilation. This
     options is enabled by default and should not be disabled since
       debugging tools relies on it.

   * `--enable-checkergcc': When enabled, NGSPICE will use the
     _Checker_ package. Checker tracks down memory errors at runtime.
          Again, this is useless for users.

   * `--enable-gc': When enabled, NGSPICE will use the Boehm-Weiser
       Conservative Garbage Collector. The garbage collector library
     is not        provided with NGSPICE, you must download and install
     it separately. Most        distributions provide a binary package
     of this library.

   * `--enable-nosqrt': When enabled, the faster code using SQRT in
       charge/capacitance calculations of bulk diodes, when the grading
           coefficients have a vaule of .5, is switched off. I think
     there is        no need to enable it.

   * `--enable-nobypass': When enabled the bypass code is not
     compiled in. Once enabled NGSPICE does not contain the code to
     bypass        recalculations of slowly changing variables. It is
     advisable to leave        this disabled since the bypass code does
     is used only if the "bypass"        option is set to `TRUE' at
     runtime.

   * `--enable-capbypass': When enabled the calculation of cbd/cbs
      in the mosfets is bypassed ifvbs/vbd voltages were unchanged.
     Better        do not enable it if you are not sure of its
     implications.

   * `--enable-capzerobypass': When enabled all the calculations
     cbd/cbs calculations if Czero is zero. It is safe to enable this
         feature.

   * `--enable-nodelimiting': Enable some experimental code that
     was intended to do Newton damping by nodes, rather than by branches
           as is currently done. The flag just turns off the branch
     limiting code        in a couple of mosfets. Obviously, do not
     enable this if you are not        working with the limiting code.

   * `--enable-predictor': When this feature is enabled, NGSPICE
     (like the orignal Spice3f) uses a predictor-corrector method for
         the numerical integration package. This feature has never
     been tested        too much, so enabling it is NOT considered safe.

   * `--enable-newtrunc': When enabled, some unfinished (?) code to
        do truncation error timestep control on node voltages (rather
     than on         charge in the devices) is activated. Casual users
     should not enable it.

   * `--enable-sense2': Use spice2 sensitivity analysis.

   * `--enable-sensdebug': Enables debug switch for sensitivity code.

   * `--enable-intnoise': If enabed, noise analysis produces an
     additional plot: the integrated noise. Users should always enable
     this.

   * `--enable-smoketest': Enables some very restrictive compilation
        flags. Useful only in development phase and, if enabled,
     probably        NGSPICE does not compile.

   * `--enable-experimental': It is possible that some untested code
        is included in stable releases. If you want to experiment with
     new        untested features, enable this option.

   * `--enable-ekv': EKV is a device model not released in source
     code form. If you have obtained the source code, you have to
     enable        this to have it compiled into NGSPICE.

   * `--with-readline': This option enables GNU Readline on NGSPICE.
         Since NGSPICE license is incompatible with GPL (which covers
     Readline        library), the code is not included compiled into
     NGSPICE by default.

   CAVEAT EMPTOR: NGSPICE, like its father Spice3f5 cannot be
considered a "black box", it is a complex numerical software whose
stability and correctness depends on many parameters. Be sure to
understand well what you enable/disable otherwise your simulations may
converge to a wrong value or do not converge at all.

   Once chosen the options to enable/disable, you will have to issue the
`configure' command followed by the options you choose, like:

   `configure --enable-intnoise --enable-nobypass
--enable-capzerobypass'

   If all goes well, all makefiles will be generated and the package is
ready to be compiled.


File: ngspice.info,  Node: Compiling NGSPICE,  Next: Supported systems,  Prev: Configuring NGSPICE,  Up: NGSPICE Compilation

5.3 Compiling NGSPICE
=====================

The reference platform for NGSPICE is a Linux system with glibc2 ang gcc
(2.95 o newer) running on the i386 architecture. If you have such a
system you can pretty sure that NGSPICE will compile correctly.

   Once configured, to compile NGSPICE `cd' into the top level directory
(if you moved from it after configuration) and issue the `make'. If you
have a multi-processor machine, you can add `-j3' to speed up
compilation.

   NGSPICE compilation takes several minutes on an average machine,
enough to let you have a lunch. Once NGSPICE has been compiled, you
have to install it issuing the command `make install'. NGSPICE will be
installed under `/usr/local/'.


File: ngspice.info,  Node: Supported systems,  Next: Platform specific issues,  Prev: Compiling NGSPICE,  Up: NGSPICE Compilation

5.4 Supported systems
=====================

NGSPICE development is carried on Linux on the i386 processor
architecture.  Compiling it under different UNIX systems should require
only trivial changes, since most of the issues will be resolved by
Autoconf. Compiling under non UNIX OSes may require major changes,
since Autoconf and other UNIX tools may not be available on those
environments.

   In the past, NGSPICE have been ported to some OSes, the table below
shows the port I am aware of:

   NETBSD

   Dan McMahill <mcmahill@mtl.mit.edu> has ported NGSPICE (starting
from rework-13) on NetBSD systems. Dan maintains a NetBSD package for
NGSPICE available at
`ftp://ftp.netbsd.org/pub/NetBSD/packages/pkgsrc/cad/ng-spice/README.html'
.

   SOLARIS 7

   Scott Griffith <skod@ises-llc.com> has compiled ngspice rework-12 on
Solaris 7 with gcc (verion 2.95.1). Some changes to the source code were
needed:

     Notes on compilation on SUN Solaris (extracted from Scott's email):
     Solaris lacks some of the functions needed by ngspice. You have to
     copy them from other GNU tools.  (Scott defines the following
     changes "some of the usual workarounds")

        * Copy `getopt.c', `getopt1.c' and `asprintf.c' from
          other GNU tools into the misc directory of the ngspice tree
          and       modify the Makefiles accordingly.

        * Change `src/maths/cmaths/test_cx_ph.c' to       `#include
          <defines.h>', because that gave me a compiler       error on
          `DBL_EPSILON'.

   WINDOWS

   Holger Vogt <holger.vogt@uni-duisburg.de> has ported NGSPICE (from
rework-14 release) to the Windows Operating System. His port relies
only on DLLs coming with Windows.

   As of Rework-16 the Windows port is integrated as part of ngspice.
It can be build under Cygwin or MinGW.

   The situation of NGSPICE ports is evolving continually, the one
above are the only I (Paolo Nenzi) am aware of. I know that there is a
intent to port NGSPICE to FreeBSD but do not know its status.

   This section will be updated in the future.


File: ngspice.info,  Node: Platform specific issues,  Prev: Supported systems,  Up: NGSPICE Compilation

5.5 Platform specific issues
============================

NGSPICE heavily relies on the floating point representation. On the i386
architecture, the floating point implementation can cause problems to
numerical software like NGSPICE. Intel i386 and later processors have
80-bit wide floating point registers in their FPU. This width is
referred ad _extended double_ precision and all the calculation are
done, internally, at that precision. Externally, the result can be used
as is or rounded to _double_ precision as defined in the IEEE754
standard for floating point, so there are two modes of operation and
the choice is left to the operating system. FreeBSD developers decided
that the FPU had to provide results conforming to IEEE745, while Linux
ones decided to take advantage of the extended precision.

   This different choice lead to slightly different results when
running the same simulation on different operating systems.
Catastrophic discrepancies arise on badly written software.


File: ngspice.info,  Node: Supported Analyses,  Next: Circuit Description,  Prev: NGSPICE Compilation,  Up: Top

6 Supported Analyses
********************

This chapter introduces the analyses available in NGSPICE.

* Menu:

* Types of Analysis::
* Analysis at Different Temperatures::
* Convergence::


File: ngspice.info,  Node: Types of Analysis,  Next: Analysis at Different Temperatures,  Prev: Supported Analyses,  Up: Supported Analyses

6.1 Types of Analysis
=====================

* Menu:

* DC Analysis::
* AC Small-Signal Analysis::
* Transient Analysis::
* Pole-Zero Analysis::
* Small-Signal Distortion Analysis::
* Sensitivity Analysis::
* Noise Analysis::


File: ngspice.info,  Node: DC Analysis,  Next: AC Small-Signal Analysis,  Prev: Types of Analysis,  Up: Types of Analysis

6.1.1 DC Analysis
-----------------

The dc analysis portion of NGSPICE determines the dc operating point of
the circuit with inductors shorted and capacitors opened.  The dc
analysis options are specified on the `.DC', `.TF', and `.OP' control
lines.A dc analysis is automatically performed prior to a transient
analysis to determine the transient initial conditions, and prior to an
ac small-signal analysis to determine the linearized, small-signal
models for nonlinear devices.  If requested, the dc small-signal value
of a transfer function (ratio of output variable to input source), input
resistance, and output resistance is also computed as a part of the dc
solution.  The dc analysis can also be used to generate dc transfer
curves: a specified independent voltage, current source, resistor or
temperature is stepped over a user-specified range and the dc output
variables are stored for each sequential source value.

   Temperature (`TEMP') and resistance sweeps have been introduced in
NGSPICE, they were not available in the original code of Spice3f5.


File: ngspice.info,  Node: AC Small-Signal Analysis,  Next: Transient Analysis,  Prev: DC Analysis,  Up: Types of Analysis

6.1.2 AC Small-Signal Analysis
------------------------------

The ac small-signal portion of NGSPICE computes the ac output variables
as a function of frequency.  The program first computes the dc
operating point of the circuit and determines linearized, small-signal
models for all of the nonlinear devices in the circuit.  The resultant
linear circuit is then analyzed over a user-specified range of
frequencies.  The desired output of an ac small-signal analysis is
usually a transfer function (voltage gain, transimpedance, etc).  If
the circuit has only one ac input, it is convenient to set that input
to unity and zero phase, so that output variables have the same value
as the transfer function of the output variable with respect to the
input.


File: ngspice.info,  Node: Transient Analysis,  Next: Pole-Zero Analysis,  Prev: AC Small-Signal Analysis,  Up: Types of Analysis

6.1.3 Transient Analysis
------------------------

The transient analysis portion of NGSPICE computes the transient output
variables as a function of time over a user-specified time interval.
The initial conditions are automatically determined by a dc analysis.
All sources which are not time dependent (for example, power supplies)
are set to their dc value.  The transient time interval is specified on
a `.TRAN' control line.


File: ngspice.info,  Node: Pole-Zero Analysis,  Next: Small-Signal Distortion Analysis,  Prev: Transient Analysis,  Up: Types of Analysis

6.1.4 Pole-Zero Analysis
------------------------

The pole-zero analysis portion of NGSPICE computes the poles and/or
zeros in the small-signal ac transfer function.  The program first
computes the dc operating point and then determines the linearized,
small-signal models for all the nonlinear devices in the circuit.  This
circuit is then used to find the poles and zeros of the transfer
function.

   Two types of transfer functions are allowed: one of the form (output
voltage)/(input voltage) and the other of the form (output
voltage)/(input current).  These two types of transfer functions cover
all the cases and one can find the poles/zeros of functions like
input/output impedance and voltage gain.  The input and output ports
are specified as two pairs of nodes.

   The pole-zero analysis works with resistors, capacitors, inductors,
linear-controlled sources, independent sources, BJTs, MOSFETs, JFETs
and diodes.  Transmission lines are not supported.

   The method used in the analysis is a sub-optimal numerical search.
For large circuits it may take a considerable time or fail to find all
poles and zeros.  For some circuits, the method becomes "lost" and
finds an excessive number of poles or zeros.


File: ngspice.info,  Node: Small-Signal Distortion Analysis,  Next: Sensitivity Analysis,  Prev: Pole-Zero Analysis,  Up: Types of Analysis

6.1.5 Small-Signal Distortion Analysis
--------------------------------------

The distortion analysis portion of NGSPICE computes steady-state
harmonic and intermodulation products for small input signal
magnitudes.  If signals of a single frequency are specified as the
input to the circuit, the complex values of the second and third
harmonics are determined at every point in the circuit.  If there are
signals of two frequencies input to the circuit, the analysis finds out
the complex values of the circuit variables at the sum and difference
of the input frequencies, and at the difference of the smaller
frequency from the second harmonic of the larger frequency.

   Distortion analysis is supported for the following nonlinear devices:
diodes (DIO), BJT, JFET, MOSFETs (levels 1, 2, 3, 4/BSIM1, 5/BSIM2, and
6) and MESFETS.  All linear devices are automatically supported by
distortion analysis.  If there are switches present in the circuit, the
analysis continues to be accurate provided the switches do not change
state under the small excitations used for distortion calculations.


File: ngspice.info,  Node: Sensitivity Analysis,  Next: Noise Analysis,  Prev: Small-Signal Distortion Analysis,  Up: Types of Analysis

6.1.6 Sensitivity Analysis
--------------------------

NGSPICE will calculate either the DC operating-point sensitivity or the
AC small-signal sensitivity of an output variable with respect to all
circuit variables, including model parameters. NGSPICE calculates the
difference in an output variable (either a node voltage or a branch
current) by perturbing each parameter of each device independently.
Since the method is a numerical approximation, the results may
demonstrate second order affects in highly sensitive parameters, or may
fail to show very low but non-zero sensitivity.  Further, since each
variable is perturb by a small fraction of its value, zero-valued
parameters are not analyized (this has the benefit of reducing what is
usually a very large amount of data).


File: ngspice.info,  Node: Noise Analysis,  Prev: Sensitivity Analysis,  Up: Types of Analysis

6.1.7 Noise Analysis
--------------------

The noise analysis portion of NGSPICE does analysis device-generated
noise for the given circuit.  When provided with an input source and an
output port, the analysis calculates the noise contributions of each
device (and each noise generator within the device) to the output port
voltage.  It also calculates the input noise to the circuit, equivalent
to the output noise referred to the specified input source.  This is
done for every frequency point in a specified range - the calculated
value of the noise corresponds to the spectral density of the circuit
variable viewed as a stationary gaussian stochastic process.

   After calculating the spectral densities, noise analysis integrates
these values over the specified frequency range to arrive at the total
noise voltage/current (over this frequency range).  This calculated
value corresponds to the variance of the circuit variable viewed as a
stationary gaussian process.


File: ngspice.info,  Node: Analysis at Different Temperatures,  Next: Convergence,  Prev: Types of Analysis,  Up: Supported Analyses

6.2 Analysis at Different Temperatures
======================================

Temperature, in NGSPICE, is a property associated to the entire circuit,
rather an analysis option. Circuit temperature has a default (nominal)
value of 27^oC (300.15 K) that can be changed using the `TNOM' option
in an `.OPTION' control line. All analyses are, thus, performed at
circuit temperature, and if you want to simulate circuit behaviour at
different temperatures you should prepare a netlist for each
temperature.

   All input data for NGSPICE is assumed to have been measured at the
circuit nominal temperature. This value can further be overridden for
any device which models temperature effects by specifying the `TNOM'
parameter on the `.model' itself.

   Individual instances may further override the circuit temperature
through the specification of `TEMP' and `DTEMP' parameters on the
instance. The two options are not independent even if you can specify
both on the instance line, the `TEMP' option overrides `DTEMP'. The
algorithm to compute instance temperature is described below:


     IF TEMP is specified THEN
             instance_temperature = TEMP
     ELSE IF
             instance_temperature = circuit_temperature + DTEMP
     END IF

   Temperature dependent support is provided for all devices except
voltage and current sources (either independent and controlled) and
BSIM models.  BSIM MOSFETs have an alternate temperature dependency
scheme which adjusts all of the model parameters before input to
NGSPICE.  For details of the BSIM temperature adjustment, see [6] and
[7].

   Temperature appears explicitly in the exponential terms of the BJT
and diode model equations.  In addition, saturation currents have a
built-in temperature dependence.  The temperature dependence of the
saturation current in the BJT models is determined by:

                             XTI
                         |T |        | E q(T  T )|
                           1            g   1  0
         I (T ) = I (T ) |--|     exp|-----------|
          S  1     S  0
                         |T |        |k (T  - T )|
                           0              1    0

   where `k' is Boltzmann's constant, `q' is the electronic charge, `E'
is the energy gap which is a model parameter, `G' and `XTI' is the
saturation current temperature exponent (also a model parameter, and
usually equal to 3).

   The temperature dependence of forward and reverse beta is according
to the formula:

                                     XTB
                                 |T |
                                   1
                   B(T ) = B(T ) |--|
                      1       0
                                 |T |
                                   0

   where `T_0' and `T_1' are in degrees Kelvin, and `XTB' is a
user-supplied model parameter.  Temperature effects on beta are carried
out by appropriate adjustment to the values of `B_F', `I_SE', `B_R',
and `I_SC' (spice model parameters `BF', `ISE', `BR', and `ISC',
respectively).

   Temperature dependence of the saturation current in the junction
diode model is determined by:

                            XTI
                            ---
                             N
                        |T |        |  E q(T  T ) |
                          1             g   1  0
        I (T ) = I (T ) |--|     exp|-------------|
         S  1     S  0
                        |T |        |N k (T  - T )|
                          0                1    0

   where `N' is the emission coefficient, which is a model parameter,
and the other symbols have the same meaning as above.  Note that for
Schottky barrier diodes, the value of the saturation current temperature
exponent, `XTI', is usually 2.

   Temperature appears explicitly in the value of junction potential,
``U'' (in NGSPICE `PHI'), for all the device models.  The temperature
dependence is determined by:

                                  | N N   |
                                     a d
                         kT       |------ |
                  U(T) = --  log        2
                          q     e |N (T)  |
                                    i

   where `k' is Boltzmann's constant, `q' is the electronic charge,
`N_a' is the acceptor impurity density, `N_d' is the donor impurity
density, `N_i' is the intrinsic carrier concentration, and `E_g' is the
energy gap.

   Temperature appears explicitly in the value of surface mobility,
`M_0' (or U_0), for the MOSFET model.  The temperature dependence is
determined by:

                               M (T )
                                0  0
                      M (T) = -------
                       0          1.5
                              | T|
                              |--|
                              |T |
                                0

   The effects of temperature on resistors, capacitor and inductors is
modeled by the formula:

                                                   2
      R(T) = R(T ) [1 + TC  (T - T ) + TC  (T - T ) ]
                0         1       0      2       0

   where `T' is the circuit temperature, `T_0' is the nominal
temperature, and `TC_1' and `TC_2' are the first and second order
temperature coefficients.


File: ngspice.info,  Node: Convergence,  Prev: Analysis at Different Temperatures,  Up: Supported Analyses

6.3 Convergence
===============

Both dc and transient solutions are obtained by an iterative process
which is terminated when both of the following conditions hold:

  1.  The nonlinear branch currents converge to within a tolerance of
     0.1% or 1 picoamp (1.0e-12 Amp), whichever is larger.

  2.  The node voltages converge to within a tolerance of 0.1% or 1
     microvolt (1.0e-6 Volt), whichever is larger.


   Although the algorithm used in NGSPICE has been found to be very
reliable, in some cases it fails to converge to a solution.  When this
failure occurs, the program terminates the job.

   Failure to converge in dc analysis is usually due to an error in
specifying circuit connections, element values, or model parameter
values.  Regenerative switching circuits or circuits with positive
feedback probably will not converge in the dc analysis unless the `OFF'
option is used for some of the devices in the feedback path, or the
`.NODESET' control line is used to force the circuit to converge to the
desired state.


File: ngspice.info,  Node: Circuit Description,  Next: Circuit Elements and Models,  Prev: Supported Analyses,  Up: Top

7 Circuit Description
*********************

* Menu:

* General Structure and Conventions::
* Basics::
* Device Models::
* Subcircuits::
* INCLUDE::


File: ngspice.info,  Node: General Structure and Conventions,  Next: Basics,  Prev: Circuit Description,  Up: Circuit Description

7.1 General Structure and Conventions
=====================================

The circuit to be analyzed is described to ngspice by a set of element
lines, which define the circuit topology and element values, and a set
of control lines, which define the model parameters and the run
controls.  The first line in the input file must be the title, and the
last line must be "`.END'".  The order of the remaining lines is
arbitrary (except, of course, that continuation lines must immediately
follow the line being continued).

   Each element in the circuit is specified by an element line that
contains the element name, the circuit nodes to which the element is
connected, and the values of the parameters that determine the
electrical characteristics of the element.  The first letter of the
element name specifies the element type.  The format for the NGSPICE
element types is given in what follows.  The strings `XXXXXXX',
`YYYYYYY', and `ZZZZZZZ' denote arbitrary alphanumeric strings.  For
example, a resistor name must begin with the letter `R' and can contain
one or more characters.  Hence, `R', `R1', `RSE', `ROUT', and `R3AC2ZY'
are valid resistor names.  Details of each type of device are supplied
in a following section.

   Fields on a line are separated by one or more blanks, a comma, an
equal (``='') sign, or a left or right parenthesis; extra spaces are
ignored.  A line may be continued by entering a ``+'' (plus) in column
1 of the following line; NGSPICE continues reading beginning with
column 2.

   A name field must begin with a letter (A through Z) and cannot
contain any delimiters.

   A number field may be an integer field (12, -44), a floating point
field (3.14159), either an integer or floating point number followed by
an integer exponent (1e-14, 2.65e3), or either an integer or a floating
point number followed by one of the following scale factors:

   `T' = 10^12  `G' = 10^9  `Meg' = 10^6  `K' = 10^3  `mil' = 25.4^-6
`m' = 10^-3  `u' = 10^-6  `n' = 10^-9  `p' = 10^-12  `f' = 10^-15

   Letters immediately following a number that are not scale factors are
ignored, and letters immediately following a scale factor are ignored.
Hence, 10, 10V, 10Volts, and 10Hz all represent the same number, and M,
MA, MSec, and MMhos all represent the same scale factor.  Note that
1000, 1000.0, 1000Hz, 1e3, 1.0e3, 1kHz, and 1k all represent the same
number.

   Nodes names may be arbitrary character strings.  The datum (ground)
node must be named `0' (zero).  Note the difference in NGSPICE where
the nodes are treated as character strings and not evaluated as numbers,
thus `0' and `00' are distinct nodes in NGSPICE but not in SPICE2.

   NGSPICE needs that the following topological constraints are
satisfied:

   * The circuit cannot contain a loop of voltage sources and/or
     inductors and cannot contain a cut-set of current sources
     and/or capacitors.

   * Each node in the circuit must have a dc path to ground.

   * Every node must have at least two connections except for
     transmission       line nodes (to permit unterminated transmission
     lines) and MOSFET       substrate nodes (which have two internal
     connections anyway).


File: ngspice.info,  Node: Basics,  Next: Device Models,  Prev: General Structure and Conventions,  Up: Circuit Description

7.2 Basics: Title Line, Comment Lines and .END Line
===================================================

* Menu:

* Title Line::
* END::
* Comments::


File: ngspice.info,  Node: Title Line,  Next: END,  Prev: Basics,  Up: Basics

7.2.1 Title Line
----------------

Examples:

          POWER AMPLIFIER CIRCUIT
          TEST OF CAM CELL

   The title line must be the first in the input file.  Its contents are
printed verbatim as the heading for each section of output.


File: ngspice.info,  Node: END,  Next: Comments,  Prev: Title Line,  Up: Basics

7.2.2 .END Line
---------------

Examples:

          .END

   The "End" line must always be the last in the input  file.   Note
that the period is an integral part of the  name.


File: ngspice.info,  Node: Comments,  Prev: END,  Up: Basics

7.2.3 Comments
--------------

General Form:

          * <any comment>

   Examples:

          * RF=1K      Gain should be 100
          * Check open-loop gain and phase margin

   The asterisk in the  first  column  indicates  that  this  line  is
a  comment  line.   Comment lines may be  placed anywhere in the
circuit description.   Note  that  NGSPICE  also considers any line
with leading white space  to be a comment.


File: ngspice.info,  Node: Device Models,  Next: Subcircuits,  Prev: Basics,  Up: Circuit Description

7.3 Device Models
=================

General form:

          .MODEL MNAME TYPE(PNAME1=PVAL1 PNAME2=PVAL2 ... )

   Examples:

          .MODEL MOD1 NPN (BF=50 IS=1E-13 VBF=50)

   Most simple circuit elements typically require only a few parameter
values.  However, some devices (semiconductor devices in particular)
that are included in NGSPICE require many parameter values.  Often, many
devices in a circuit are defined by the same set of device model
parameters.  For these reasons, a set of device model parameters is
defined on a separate .MODEL line and assigned a unique model name.  The
device element lines in NGSPICE then refer to the model name.

   For these more complex device types, each device element line
contains the device name, the nodes to which the device is connected,
and the device model name.  In addition, other optional parameters may
be specified for some devices: geometric factors and an initial
condition (see the following section on Transistors and Diodes for more
details).

   MNAME in the above is the model name, and type is one of the
following fifteen types:

`R'
     Semiconductor resistor model

`C'
     Semiconductor capacitor model

`L'
     Inductor model

`SW'
     Voltage controlled switch

`CSW'
     Current controlled switch

`URC'
     Uniform distributed RC model

`LTRA'
     Lossy transmission line model

`D'
     Diode model

`NPN'
     NPN BJT model

`PNP'
     PNP BJT model

`NJF'
     N-channel JFET model

`PJF'
     P-channel JFET model

`NMOS'
     N-channel MOSFET model

`PMOS'
     P-channel MOSFET model

`NMF'
     N-channel MESFET model

`PMF'
     P-channel MESFET model

   Parameter values are defined by appending the parameter name
followed by an equal sign and the parameter value.  Model parameters
that are not given a value are assigned the default values given below
for each model type.  Models, model parameters, and default values are
listed in the next section along with the description of device element
lines.


File: ngspice.info,  Node: Subcircuits,  Next: INCLUDE,  Prev: Device Models,  Up: Circuit Description

7.4 Subcircuits
===============

A subcircuit that consists of NGSPICE elements can be defined and
referenced in a fashion similar to device models.  The subcircuit is
defined in the input file by a grouping of element lines; the program
then automatically inserts the group of elements wherever the subcircuit
is referenced.  There is no limit on the size or complexity of
subcircuits, and subcircuits may contain other subcircuits.  An example
of subcircuit usage is given in Appendix A.

* Menu:

* SUBCKT::
* ENDS::
* Subcircuit Calls::


File: ngspice.info,  Node: SUBCKT,  Next: ENDS,  Prev: Subcircuits,  Up: Subcircuits

7.4.1 .SUBCKT Line
------------------

General form:

          .SUBCKT subnam N1 <N2 N3 ...>

   Examples:

          .SUBCKT OPAMP 1 2 3 4

   A circuit definition is begun with a .SUBCKT line.  SUBNAM is the
subcircuit name, and N1, N2, ... are the external nodes, which cannot
be zero.  The group of element lines which immediately follow the
.SUBCKT line define the subcircuit.  The last line in a subcircuit
definition is the .ENDS line (see below).  Control lines may not appear
within a subcircuit definition; however, subcircuit definitions may
contain anything else, including other subcircuit definitions, device
models, and subcircuit calls (see below).  Note that any device models
or subcircuit definitions included as part of a subcircuit definition
are strictly local (i.e., such models and definitions are not known
outside the subcircuit definition).  Also, any element nodes not
included on the .SUBCKT line are strictly local, with the exception of
0 (ground) which is always global.


File: ngspice.info,  Node: ENDS,  Next: Subcircuit Calls,  Prev: SUBCKT,  Up: Subcircuits

7.4.2 ENDS Line
---------------

General form:

          .ENDS <SUBNAM>

   Examples:

          .ENDS OPAMP

   The "Ends" line must be the last one for any subcircuit definition.
The subcircuit name, if included, indicates which subcircuit definition
is being terminated; if omitted, all subcircuits being defined are
terminated.  The name is needed only when nested subcircuit definitions
are being made.


File: ngspice.info,  Node: Subcircuit Calls,  Prev: ENDS,  Up: Subcircuits

7.4.3 Subcircuit Calls
----------------------

General form:

          XYYYYYYY N1 <N2 N3 ...> SUBNAM

   Examples:

          X1 2 4 17 3 1 MULTI

   Subcircuits are used in NGSPICE by specifying pseudo-elements
beginning with the letter X, followed by the circuit nodes to be used
in expanding the subcircuit.


File: ngspice.info,  Node: INCLUDE,  Prev: Subcircuits,  Up: Circuit Description

7.5 INCLUDE
===========

General form:

       .INCLUDE filename

   Examples:

       .INCLUDE /users/spice/common/wattmeter.cir

   Frequently, portions of circuit descriptions will be reused in
several input files, particularly with common models and subcircuits.
In any ngspice input file, the ".include" line may be used to copy some
other file as if that second file appeared in place of the ".include"
line in the original file.  There is no restriction on the file name
imposed by ngspice beyond those imposed by the local operating system.


File: ngspice.info,  Node: Circuit Elements and Models,  Next: Analyses and Output Control,  Prev: Circuit Description,  Up: Top

8 Circuit Elements and Models
*****************************

Data fields that are enclosed in less-than and greater-than signs ('<
>') are optional.  All indicated punctuation (parentheses, equal signs,
etc.) is optional but indicate the presence of any delimiter.  Further,
future implementations may require the punctuation as stated.  A
consistent style adhering to the punctuation shown here makes the input
easier to understand.  With respect to branch voltages and currents,
NGSPICE uniformly uses the associated reference convention (current
flows in the direction of voltage drop).

* Menu:

* General options and information::
* Elementary Devices::
* Voltage and Current Sources::
* Transmission Lines::
* Transistors and Diodes::


File: ngspice.info,  Node: General options and information,  Next: Simulating more devices in parallel,  Prev: Circuit Elements and Models,  Up: Circuit Elements and Models

8.1 General options and information
===================================

* Menu:

* Simulating more devices in parallel::
* Technology scaling::
* Model binning::


File: ngspice.info,  Node: Simulating more devices in parallel,  Next: Technology scaling,  Prev: General options and information,  Up: General options and information

8.1.1 Simulating more devices in parallel
-----------------------------------------

If you need to simulate more devices of the same kind in parallel, you
can use the `m' (often called parallel multiplier) option which is
available for all instances except transmission lines and sources (both
independent and controlled).

   The parallel multiplier is implemented by multiplying by the value of
`m' the element's matrix stamp, thus it cannot be used to accurately
simulate larger devices in integrated circuits.

   The netlist below show how to correctly use the parallel multiplier:

     Multiple devices

     d1  2  0 mydiode  m=10

     d01 1  0 mydiode
     d02 1  0 mydiode
     d03 1  0 mydiode
     d04 1  0 mydiode
     d05 1  0 mydiode
     d06 1  0 mydiode
     d07 1  0 mydiode
     d08 1  0 mydiode
     d09 1  0 mydiode
     d10 1  0 mydiode

     ...

   The `d1' instance connected between nodes 2 and 0  is equivalent to
the parallel `d01-d10' connected between 1 and 0.


File: ngspice.info,  Node: Technology scaling,  Next: Model binning,  Prev: Simulating more devices in parallel,  Up: General options and information

8.1.2 Technology scaling
------------------------

Still to be implemented and written.


File: ngspice.info,  Node: Model binning,  Next: Elementary Devices,  Prev: Technology scaling,  Up: General options and information

8.1.3 Model binning
-------------------

Still to be implemented and written.


File: ngspice.info,  Node: Elementary Devices,  Next: Resistors,  Prev: Model binning,  Up: Circuit Elements and Models

8.2 Elementary Devices
======================

* Menu:

* Resistors::
* Semiconductor Resistors::
* Semiconductor Resistor Model (R)::
* Capacitors::
* Semiconductor Capacitors::
* Semiconductor Capacitor Model (C)::
* Inductors::
* Inductor model::
* Coupled (Mutual) Inductors::
* Switches::
* Switch Model (SW/CSW)::


File: ngspice.info,  Node: Resistors,  Next: Semiconductor Resistors,  Prev: Elementary Devices,  Up: Elementary Devices

8.2.1 Resistors
---------------

General form:

       RXXXXXXX n+ n- value <ac=val> <m=val> <scale=val> <temp=val>
       +        <dtemp=val> <noisy=0|1>

   Examples:

       R1 1 2 100
       RC1 12 17 1K
       R2 5 7 1K ac=2K
       RL 1 4 2K m=2

   Ngspice has a fairly complex model for resistors. It can simulate
both discrete and semiconductor resistors. Semiconductor resistors in
ngspice means: resistors described by geometrical parameters. So, do
not expect detailed modelling of semiconductor effects.

   `n+' and `n-' are the two element nodes, `value' is the resistance
(in ohms) and may be positive or negative but not zero.

   HINT: If you need to simulate very small resistors (0.001 Ohm or
less), you should use CCVS (transresistance), it is less efficient but
improves overall numerical accuracy. Think about that a small resistance
is a large conductance.

   Ngspice can assign a resistor instance a different value for AC
analysis, specified using the `ac' keyword. This value must not be zero
as described above. The AC resistance is used in AC analysis only (not
Pole-Zero nor noise).  If you do not specify the `ac' parameter, it is
defaulted to `value'.

   If you want to simulate temperature dependence of a resistor, you
need to specify its temperature coefficients, using a `.model' line,
like in the example below:

       RE1 1 2 700 std dtemp=5

       .MODEL std tc1=0.001

   Instance temperature is useful even if resistance does not varies
with it, since the thermal noise generated by a resistor depends on its
absolute temperature.

   Resistors in ngspice generates two different noises: thermal and
flicker. While thermal noise is always generated in the resistor, to
add a flicker noise source you have to add a `.model' card defining the
flicker noise parameters.  It is possible to simulate resistors that do
not generate any kind of noise using the `noisy' keyword  and assigning
zero to it, as in the following example:

       Rmd 134 57 1.5k noisy=0

   Ngspice calculates the nominal resistance as described below:

                             Rnom = value * scale / m
     			Racnom = ac * scale / m

   If you are interested in temperature effects or noise equations, read
the following section on semiconductor resistors.


File: ngspice.info,  Node: Semiconductor Resistors,  Next: Semiconductor Resistor Model (R),  Prev: Resistors,  Up: Elementary Devices

8.2.2 Semiconductor Resistors
-----------------------------

General form:

       RXXXXXXX n+ n- <value> <mname> <l=length> <w=width> <temp=val>
       +        <dtemp=val> m=<val> <ac=val> <scale=val> <noisy = 0|1>

   Examples:

       RLOAD 2 10 10K
       RMOD 3 7 RMODEL L=10u W=1u

   This is the more general form of the resistor presented before
(*note Resistors::) and allows the modelling of temperature effects and
for the calculation of the  actual resistance value from strictly
geometric information and the specifications of the process.  If
`value' is specified, it overrides the geometric information and
defines the resistance.  If `mname' is specified, then the resistance
may be calculated from the process information in the model `mname' and
the given `length' and `width'. If `value' is not specified, then
`mname' and `length' must be specified.  If `width' is not specified,
then it is taken from the default width given in the model.

   The (optional) `temp' value is the temperature at which this device
is to operate, and overrides the temperature specification on the
`.option' control line and the value specified in `dtemp'.


File: ngspice.info,  Node: Semiconductor Resistor Model (R),  Next: Capacitors,  Prev: Semiconductor Resistors,  Up: Elementary Devices

8.2.3 Semiconductor Resistor Model (R)
--------------------------------------

The resistor model consists of process-related device data that allow
the resistance to be calculated from geometric information and to be
corrected for temperature.  The parameters available are:

name     parameter                           units       default   example
TC1      first order temperature coeff.      ohm/^oC     0.0       
TC2      second order temperature coeff.     ohm/^oC^2   0.0       
RSH      sheet resistance                    ohm/[]      -         50
DEFW     default width                       meters      1e-6      2e-6
NARROW   narrowing due to side etching       meters      0.0       1e-7
SHORT    shortening due to side etching      meters      0.0       1e-7
TNOM     parameter measurement temperature   ^oC         27        50
KF       flicker noise coefficient           -           0.0       1e-25
AF       flicker noise exponent              -           0.0       1.0

   The sheet resistance is used with the narrowing parameter and `l'
and `w' from the resistor device to determine the nominal resistance by
the formula:

                                l -  SHORT
                     Rnom = rsh ----------
                                w - NARROW

   `DEFW' is used to supply a default value for `w' if one is not
specified for the device.  If either `rsh' or `l' is not specified,
then the standard default resistance value of 1k Ohm is used.  `TNOM'
is used to override the circuit-wide value given on the `.options'
control line where the parameters of this model have been measured at a
different temperature.

   After the nominal resistance is calculated, it is adjusted for
temperature by the formula:

                                                          2
       R(T) = R(TNOM) [1 + TC  (T - TNOM) + TC  (T - TNOM) ]
                             1                2
       where R(TNOM) = Rnom or Racnom

   In the above formula, `T' represents the instance temperature, which
can be explicitly using the `temp' keyword or os calculated using the
circuit temperature and `dtemp', if present.

   If both `temp' and `dtemp' are specified, the latter is ignored.

   Ngspice improves spice's resistors noise model, adding flicker noise
(1/f) to it and the `noisy' keyword to simulate noiseless resistors.
The thermal noise in resistors is modelled according to the equation:


                              ___
     			  2  4 k T
     			 i = ----- df
     			  r    R

   where "k" is the Boltzmann's constant, and "T" the instance
temperature.

   Flicker noise model is:


                               ____        AF
     			   2     KF Ir
     			  i   = ------- df
     			   Rfn     f

   A small list of sheet resistances (in Ohm/[]) for conductors is
shown below.  The table represents typical values for MOS processes in
the 0.5 - 1 um range. The table is taken from: _N. Weste, K. Eshraghian
- Principles of CMOS VLSI Design 2nd Edition,  Addison Wesley_.

Material                                 Min.        Typical     Max.
Intermetal (metal1 - metal2)             0.005       0.007       0.1
Top-metal (metal 3)                      0.003       0.004       0.05
Polysilicon                              15          20          30
Silicide                                 2           3           6
Diffusion(n+,p+)                         10          25          100
Silicided diffusion                      2           4           10
n-well                                   1000        2000        5000


File: ngspice.info,  Node: Capacitors,  Next: Semiconductor Capacitors,  Prev: Semiconductor Resistor Model (R),  Up: Elementary Devices

8.2.4 Capacitors
----------------

General form:

       CXXXXXXX n+ n- <value> <mname> <m=val> <scale=val> <temp=val>
       +        <dtemp=val> <ic=init_condition>

   Examples:

       CBYP 13 0 1UF
       COSC 17 23 10U IC=3V

   Ngspice provides a detailed model for capacitors.  Capacitors in the
netlist can be specified giving their capacitance or their geometrical
and physical characteristics. Following the original spice3
"convention", capacitors specified by their geometrical or physical
characteristics are called "semiconductor capacitors" and are described
in the next section.

   In this first form `n+' and `n-' are the positive and negative
element nodes, respectively and  `value' is the capacitance in Farads.

   Capacitance can be specified in the instance line as in the examples
above or in a `.model' line, as in the example below:

       C1 15 5 cstd
       C2  2 7 cstd

       .model cstd C cap=3n

   Both capacitors have a capacitance of 3nF.

   If you want to simulate temperature dependence of a capacitor, you
need to specify its temperature coefficients, using a `.model' line,
like in the example below:

       CEB 1 2 1u cap1 dtemp=5

       .MODEL cap1 C tc1=0.001

   The (optional) initial condition is the initial (timezero) value of
capacitor voltage (in Volts).  Note that the initial conditions (if any)
apply 'only' if the `uic' option is specified on the `.tran' control
line.

   Ngspice calculates the nominal capacitance as described below:

                             Cnom = value * scale * m


File: ngspice.info,  Node: Semiconductor Capacitors,  Next: Semiconductor Capacitor Model (C),  Prev: Capacitors,  Up: Elementary Devices

8.2.5 Semiconductor Capacitors
------------------------------

General form:

       CXXXXXXX n+ n- <value> <mname> <l=length> <w=width> <m=val>
       +        <scale=val> <temp=val> <dtemp=val> <ic=init_condition>

   Examples:

       CLOAD 2 10 10P
       CMOD 3 7 CMODEL L=10u W=1u

   This is the more general form of the Capacitor presented in section
(*note Capacitors::), and allows for the calculation of the actual
capacitance value from strictly geometric information and the
specifications of the process.  If `value' is specified, it defines the
capacitance and both process and geometrical information are discarded.
If `value' is not specified, the capacitance is calculated from
information contained model `mname' and the given length and width
(`l', `w' keywords, respectively).  It is possible to specify  `mname'
only, without geometrical dimensions and set the capacitance in the
`.model' line (*note Capacitors::).


File: ngspice.info,  Node: Semiconductor Capacitor Model (C),  Next: Inductors,  Prev: Semiconductor Capacitors,  Up: Elementary Devices

8.2.6 Semiconductor Capacitor Model (C)
---------------------------------------

The capacitor model contains process information that may be used to
compute the capacitance from strictly geometric information.

name     parameter                           units     default   example
CAP      model capacitance                   F         0.0       1e-6
CJ       junction bottom capacitance         F/meters^2-         5e-5
CJSW     junction sidewall capacitance       F/meters  -         2e-11
DEFW     default device width                meters    1e-6      2e-6
DEFL     default device length               meters    0.0       1e-6
NARROW   narrowing due to side etching       meters    0.0       1e-7
SHORT    shorting due to side etching        meters    0.0       1e-7
TC1      first order temperature coeff.      F/^oC     0.0       0.001
TC2      second order temperature coeff.     F/^oC^2   0.0       0.0001
TNOM     parameter measurement temperature   ^oC       27        50
DI       relative dielectric constant        F/m       0.0       1
THICK    insulator thickness                 meters    0.0       1e-9

   The capacitor has a capacitance computed as:

   If `value' is specified on the instance line then

                        Cnom = value * scale * m

   If model capacitance is specified then

                        Cnom = CAP * scale * m

   If neither `value' nor `CAP' are specified, then geometrical and
physical parameters are take into account:

                 C0 = CJ (l - NARROW) (w - NARROW) +
                        2 CJSW (l - SHORT + w -  NARROW)

   `CJ' can be explicitly given on the `.model' line or calculated by
physical parameters. When `CJ' is not given, is calculated as:

   If `THICK' is not zero:

                             DI * eps
     			        0
                        CJ = ---------   if DI is specified
     		         THICK

                              eps
     			    SiO
     			       2
                        CJ = ---------   if DI is not specified
     		         THICK

     with:

     eps =    8.854214871e-12 F/m
        0

     eps    = 3.4531479969e-11 F/m
        SiO
           2

                        Cnom = C0 * scale * m

   After the nominal capacitance is calculated, it is adjusted for
temperature by the formula:

                                                          2
       C(T) = C(TNOM) [1 + TC  (T - TNOM) + TC  (T - TNOM) ]
                             1                2
       where C(TNOM) = Cnom

   In the above formula, `T' represents the instance temperature, which
can be explicitly using the `temp' keyword or os calculated using the
circuit temperature and `dtemp', if present.


File: ngspice.info,  Node: Inductors,  Next: Inductor model,  Prev: Semiconductor Capacitor Model (C),  Up: Elementary Devices

8.2.7 Inductors
---------------

General form:

       LYYYYYYY n+ n- <value> <mname> <nt=val> <m=val> <scale=val> <temp=val>
       +        <dtemp=val> <ic=init_condition>

   Examples:

          LLINK 42 69 1UH
          LSHUNT 23 51 10U IC=15.7MA

   The inductor device implemented into ngspice has many enhancements
over the original one. `n+' and `n-' are the positive and negative
element nodes, respectively. `value' is the inductance in Henries.

   Inductance can be specified in the instance line as in the examples
above or in a `.model' line, as in the example below:

       L1 15 5 indmod1
       L2  2 7 indmod1

       .model indmod1 L ind=3n

   Both inductors have an inductance of 3nH.

   The `nt' is used in conjunction with a `.model' line, and is used to
specify the number of turns of the inductor.

   If you want to simulate temperature dependence of an inductor, you
need to specify its temperature coefficients, using a `.model' line,
like in the example below:

       Lload 1 2 1u ind1 dtemp=5

       .MODEL ind1 L tc1=0.001

   The (optional) initial condition is the initial (timezero) value of
inductor current (in Amps) that flows from `n+', through the inductor,
to `n-'.  Note that the initial conditions (if any) apply only if the
`UIC' option is specified on the `.tran' analysis line.

   Ngspice calculates the nominal inductance as described below:

                             Lnom = value * scale / m


File: ngspice.info,  Node: Inductor model,  Next: Coupled (Mutual) Inductors,  Prev: Inductors,  Up: Elementary Devices

8.2.8 Inductor model
--------------------

The inductor model contains physical and geometrical information that
may be used to compute the inductance of some common topologies like
solenoids and toroids, wound in air or other material with constant
magnetic permeability.

name        parameter                     units          default example
IND         model inductance              H              0.0     1e-3
CSECT       Cross section                 meters^2       0.0     1e-3
LENGTH      Length                        meters         0.0     1e-2
TC1         first order temperature       F/^oC          0.0     0.001
            coeff.                                               
TC2         second order temperature      F/^oC^2        0.0     0.0001
            coeff.                                               
TNOM        parameter measurement         ^oC            27      50
            temperature                                          
NT          number of turns               -              0.0     10
MU          relative magnetic             H/meters       0.0     -
            permeability                                         

   The inductor has an inductance computed as:

   If `value' is specified on the instance line then

                        Lnom = value * scale / m

   If model inductance is specified then

                        Lnom = IND * scale / m

   If neither `value' nor `IND' are specified, then geometrical and
physical parameters are take into account. In the following formulas
`NT' refers to both instance and model parameter (instance parameter
overrides model parameter):

   If `LENGTH' is not zero:

                                   2
                       MU * mu * NT * CSECT
     			 0
                Lnom = --------------------   if MU is specified
                             LENGTH


                              2
                       mu * NT * CSECT
                         0
                Lnom = ---------------   if MU is not specified
     		      LENGTH

     with:

     mu =  1.25663706143592e-6  H/m
       0

   After the nominal inductance is calculated, it is adjusted for
temperature by the formula:

                                                          2
       L(T) = L(TNOM) [1 + TC  (T - TNOM) + TC  (T - TNOM) ]
                             1                2
       where L(TNOM) = Lnom

   In the above formula, `T' represents the instance temperature, which
can be explicitly using the `temp' keyword or calculated using the
circuit temperature and `dtemp', if present.


File: ngspice.info,  Node: Coupled (Mutual) Inductors,  Next: Switches,  Prev: Inductor model,  Up: Elementary Devices

8.2.9 Coupled (Mutual) Inductors
--------------------------------

General form:

       KXXXXXXX LYYYYYYY LZZZZZZZ value

   Examples:

       K43 LAA LBB 0.999
       KXFRMR L1 L2 0.87

   LYYYYYYY and LZZZZZZZ are the names of the two coupled inductors, and
`value' is the coefficient of coupling, K, which must be greater than 0
and less than or equal to 1.  Using the 'dot' convention, place a 'dot'
on the first node of each inductor.


File: ngspice.info,  Node: Switches,  Next: Switch Model (SW/CSW),  Prev: Coupled (Mutual) Inductors,  Up: Elementary Devices

8.2.10 Switches
---------------

General form:

          SXXXXXXX N+ N- NC+ NC- MODEL <ON><OFF>
          WYYYYYYY N+ N- VNAM MODEL <ON><OFF>

   Examples:

          s1 1 2 3 4 switch1 ON
          s2 5 6 3 0 sm2 off
          Switch1 1 2 10 0 smodel1
          w1 1 2 vclock switchmod1
          W2 3 0 vramp sm1 ON
          wreset 5 6 vclck lossyswitch OFF

   Nodes 1 and 2 are the nodes between which the switch terminals are
connected.  The model name is mandatory while the initial conditions are
optional.  For the voltage controlled switch, nodes 3 and 4 are the
positive and negative controlling nodes respectively.  For the current
controlled switch, the controlling current is that through the specified
voltage source.  The direction of positive controlling current flow is
from the positive node, through the source, to the negative node.


File: ngspice.info,  Node: Switch Model (SW/CSW),  Prev: Switches,  Up: Elementary Devices

8.2.11 Switch Model (SW/CSW)
----------------------------

The switch model allows an almost ideal switch to be described in
NGSPICE.  The switch is not quite ideal, in that the resistance can not
change from 0 to infinity, but must always have a finite positive
value.  By proper selection of the on and off resistances, they can be
effectively zero and infinity in comparison to other circuit elements.
The parameters available are:

name        parameter                     units          default switch
VT          threshold voltage             Volts          0.0     S
IT          threshold current             Amps           0.0     W
VH          hysteresis voltage            Volts          0.0     S
IH          hysteresis current            Amps           0.0     W
RON         on resistance                 Z              1.0     both
ROFF        off resistance                Z              1/GMIN* both

   *(See the .OPTIONS control line for a description of GMIN, its
default value results in an off-resistance of 1.0e+12 ohms.)

   The use of an ideal element that is highly nonlinear such as a switch
can cause large discontinuities to occur in the circuit node voltages.
A rapid change such as that associated with a switch changing state can
cause numerical roundoff or tolerance problems leading to erroneous
results or timestep difficulties.  The user of switches can improve the
situation by taking the following steps:

   First, it is wise to set ideal switch impedances just high or low
enough to be negligible with respect to other circuit elements.  Using
switch impedances that are close to "ideal" in all cases aggravates the
problem of discontinuities mentioned above.  Of course, when modelling
real devices such as MOSFETS, the on resistance should be adjusted to a
realistic level depending on the size of the device being modelled.

   If a wide range of ON to OFF resistance must be used in the switches
(ROFF/RON >1e+12), then the tolerance on errors allowed during transient
analysis should be decreased by using the .OPTIONS control line and
specifying TRTOL to be less than the default value of 7.0.  When
switches are placed around capacitors, then the option CHGTOL should
also be reduced.  Suggested values for these two options are 1.0 and
1e-16 respectively.  These changes inform NGSPICE to be more careful
around the switch points so that no errors are made due to the rapid
change in the circuit.


File: ngspice.info,  Node: Voltage and Current Sources,  Next: Transmission Lines,  Up: Circuit Elements and Models

8.3 Voltage and Current Sources
===============================

* Menu:

* Independent Sources::
* Linear Dependent Sources::
* Non-linear Dependent Sources::


File: ngspice.info,  Node: Independent Sources,  Next: Linear Dependent Sources,  Prev: Voltage and Current Sources,  Up: Voltage and Current Sources

8.3.1 Independent Sources
-------------------------

General form:

          VXXXXXXX N+ N- <<DC> DC/TRAN VALUE> <AC <ACMAG <ACPHASE>>>
          +       <DISTOF1 <F1MAG <F1PHASE>>> <DISTOF2 <F2MAG <F2PHASE>>>
          IYYYYYYY N+ N- <<DC> DC/TRAN VALUE> <AC <ACMAG <ACPHASE>>>
          +       <DISTOF1 <F1MAG <F1PHASE>>> <DISTOF2 <F2MAG <F2PHASE>>>

   Examples:

          VCC 10 0 DC 6
          VIN 13 2 0.001 AC 1 SIN(0 1 1MEG)
          ISRC 23 21 AC 0.333 45.0 SFFM(0 1 10K 5 1K)
          VMEAS 12 9
          VCARRIER 1 0 DISTOF1 0.1 -90.0
          VMODULATOR 2 0 DISTOF2 0.01
          IIN1 1 5 AC 1 DISTOF1 DISTOF2 0.001

   N+ and N- are the positive and negative nodes, respectively.  Note
that voltage sources need not be grounded.  Positive current is assumed
to flow from the positive node, through the source, to the negative
node.  A current source of positive value forces current to flow out of
the N+ node, through the source, and into the N- node.  Voltage
sources, in addition to being used for circuit excitation, are the
'ammeters' for NGSPICE, that is, zero valued voltage sources may be
inserted into the circuit for the purpose of measuring current.  They
of course have no effect on circuit operation since they represent
short-circuits.

   DC/TRAN is the dc and transient analysis value of the source.  If the
source value is zero both for dc and transient analyses, this value may
be omitted.  If the source value is time-invariant (e.g., a power
supply), then the value may optionally be preceded by the letters DC.

   ACMAG is the ac magnitude and ACPHASE is the ac phase.  The source is
set to this value in the ac analysis.  If ACMAG is omitted following the
keyword AC, a value of unity is assumed.  If ACPHASE is omitted, a value
of zero is assumed.  If the source is not an ac small-signal input, the
keyword AC and the ac values are omitted.

   DISTOF1 and DISTOF2 are the keywords that specify that the
independent source has distortion inputs at the frequencies F1 and F2
respectively (see the description of the .DISTO control line).  The
keywords may be followed by an optional magnitude and phase.  The
default values of the magnitude and phase are 1.0 and 0.0 respectively.

   Any independent source can be assigned a time-dependent value for
transient analysis.  If a source is assigned a time-dependent value, the
time-zero value is used for dc analysis.  There are five independent
source functions: pulse, exponential, sinusoidal, piece-wise linear, and
single-frequency FM.  If parameters other than source values are omitted
or set to zero, the default values shown are assumed.  (TSTEP is the
printing increment and TSTOP is the final time (see the .TRAN control
line for explanation)).

* Menu:

* Pulse::
* Sinusoidal::
* Exponential::
* Piece-Wise Linear::
* Single-Frequency FM::


File: ngspice.info,  Node: Pulse,  Next: Sinusoidal,  Prev: Independent Sources,  Up: Independent Sources

8.3.1.1 Pulse
.............

General form:

          PULSE(V1 V2 TD TR TF PW PER)

   Examples:

          VIN 3 0 PULSE(-1 1 2NS 2NS 2NS 50NS 100NS)

parameter                default value            units
V1 (initial value)                                Volts or Amps
V2 (pulsed value)                                 Volts or Amps
TD (delay time)          0.0                      seconds
TR (rise time)           TSTEP                    seconds
TF (fall time)           TSTEP                    seconds
PW (pulse width)         TSTOP                    seconds
PER(period)              TSTOP                    seconds

   A single pulse so specified is described by the following table:

time                   value
0                      V1
TD                     V1
TD+TR                  V2
TD+TR+PW               V2
TD+TR+PW+TF            V1
TSTOP                  V1

   Intermediate points are determined by linear interpolation.


File: ngspice.info,  Node: Sinusoidal,  Next: Exponential,  Prev: Pulse,  Up: Independent Sources

8.3.1.2 Sinusoidal
..................

General form:

          SIN(VO VA FREQ TD THETA)

   Examples:

          VIN 3 0 SIN(0 1 100MEG 1NS 1E10)

parameters             default value          units
VO (offset)                                   Volts or Amps
VA (amplitude)                                Volts or Amps
FREQ (frequency)       1/TSTOP                Hz
TD (delay)             0.0                    seconds
THETA (damping         0.0                    1/seconds
factor)                                       

   The shape of the waveform is described by the following table:

     time          value
     ------------------------------------------------------------
     0 to TD       VO
                            -(t - TD)THETA
     TD to TSTOP   VO + VA e               sin(2 J FREQ (t + TD))


File: ngspice.info,  Node: Exponential,  Next: Piece-Wise Linear,  Prev: Sinusoidal,  Up: Independent Sources

8.3.1.3 Exponential
...................

General Form:

          EXP(V1 V2 TD1 TAU1 TD2 TAU2)

   Examples:

          VIN 3 0 EXP(-4 -1 2NS 30NS 60NS 40NS)

     parameter                   default value   units
     ---------------------------------------------------------
     V1   (initial value)                        Volts or Amps
     V2   (pulsed value)                         Volts or Amps
     TD1  (rise delay time)      0.0             seconds
     TAU1 (rise time constant)   TSTEP           seconds
     TD2  (fall delay time)      TD1+TSTEP       seconds
     TAU2 (fall time constant)   TSTEP           seconds

   The shape of the waveform is described by the following table:

     time           value
     ---------------------------------------------------------------------
     0 to TD1      V1
                                |    -(t - TD1)|
     TD1 to TD2    V1 + (V2-V1).|1-e ----------|
                                |       TAU1   |

                                |    -(t - TD1)|           |   -(t - TD2)|
     TD2 to TSTOP  V1 + (V2-V1).|1-e ----------| + (V1-V2).|1-e ---------|
                                |        TAU1  |           |       TAU2  |


File: ngspice.info,  Node: Piece-Wise Linear,  Next: Single-Frequency FM,  Prev: Exponential,  Up: Independent Sources

8.3.1.4 Piece-Wise Linear
.........................

General Form:

          PWL(T1 V1 <T2 V2 T3 V3 T4 V4 ...>)

   Examples:

          VCLOCK 7 5 PWL(0 -7 10NS -7 11NS -3 17NS -3 18NS -7 50NS -7)

   Each pair of values (Ti, Vi) specifies that the value of the source
is Vi (in Volts or Amps) at time=Ti.  The value of the source at
intermediate values of time is determined by using linear interpolation
on the input values.


File: ngspice.info,  Node: Single-Frequency FM,  Prev: Piece-Wise Linear,  Up: Independent Sources

8.3.1.5 Single-Frequency FM
...........................

General Form:

          SFFM(VO VA FC MDI FS)

   Examples:

          V1 12 0 SFFM(0 1M 20K 5 1K)

     parameter                 default value   units
     ------------------------------------------------------
     VO  (offset)                              Volts or Amps
     VA  (amplitude)                           Volts or Amps
     FC  (carrier frequency)   1/TSTOP         Hz
     MDI (modulation index)
     FS  (signal frequency)    1/TSTOP         Hz

   The shape of the waveform is described by the following equation:

                       |                            |
       V(t)=V  + V  sin 2 J FC t + MDI sin(2 J FS t)
             O    A    |                            |


File: ngspice.info,  Node: Linear Dependent Sources,  Next: Non-linear Dependent Sources,  Prev: Independent Sources,  Up: Voltage and Current Sources

8.3.2 Linear Dependent Sources
------------------------------

NGSPICE allows circuits to contain linear dependent sources
characterized by any of the four equations

        i = g v          v = e v          i = f i          v = h i

   where g, e, f, and h are constants representing transconductance,
voltage gain, current gain, and transresistance, respectively.

* Menu:

* Linear Voltage-Controlled Current Sources::
* Linear Voltage-Controlled Voltage Sources::
* Linear Current-Controlled Current Sources::
* Linear Current-Controlled Voltage Sources::


File: ngspice.info,  Node: Linear Voltage-Controlled Current Sources,  Next: Linear Voltage-Controlled Voltage Sources,  Prev: Linear Dependent Sources,  Up: Linear Dependent Sources

8.3.2.1 Linear Voltage-Controlled Current Sources
.................................................

General form:

          GXXXXXXX N+ N- NC+ NC- VALUE

   Examples:

          G1 2 0 5 0 0.1MMHO

   N+ and N- are the positive and negative nodes, respectively.  Current
flow is from the positive node, through the source, to the negative
node.  NC+ and NCare the positive and negative controlling nodes,
respectively.  VALUE is the transconductance (in mhos).


File: ngspice.info,  Node: Linear Voltage-Controlled Voltage Sources,  Next: Linear Current-Controlled Current Sources,  Prev: Linear Voltage-Controlled Current Sources,  Up: Linear Dependent Sources

8.3.2.2 Linear Voltage-Controlled Voltage Sources
.................................................

General form:

          EXXXXXXX N+ N- NC+ NC- VALUE

   Examples:

          E1 2 3 14 1 2.0

   N+ is the positive node, and N- is the negative node.  NC+ and NC-
are the positive and negative controlling nodes, respectively.  VALUE
is the voltage gain.


File: ngspice.info,  Node: Linear Current-Controlled Current Sources,  Next: Linear Current-Controlled Voltage Sources,  Prev: Linear Voltage-Controlled Voltage Sources,  Up: Linear Dependent Sources

8.3.2.3 Linear Current-Controlled Current Sources
.................................................

General form:

          FXXXXXXX N+ N- VNAM VALUE

   Examples:

          F1 13 5 VSENS 5

   N+ and N- are the positive and negative nodes, respectively.  Current
flow is from the positive node, through the source, to the negative
node.  VNAM is the name of a voltage source through which the
controlling current flows.  The direction of positive controlling
current flow is from the positive node, through the source, to the
negative node of VNAM.  VALUE is the current gain.


File: ngspice.info,  Node: Linear Current-Controlled Voltage Sources,  Prev: Linear Current-Controlled Current Sources,  Up: Linear Dependent Sources

8.3.2.4 Linear Current-Controlled Voltage Sources
.................................................

General form:

          HXXXXXXX N+ N- VNAM VALUE

   Examples:

          HX 5 17 VZ 0.5K

   N+ and N- are the positive and negative nodes, respectively.  VNAM is
the name of a voltage source through which the controlling current
flows.  The direction of positive controlling current flow is from the
positive node, through the source, to the negative node of VNAM.  VALUE
is the transresistance (in ohms).


File: ngspice.info,  Node: Non-linear Dependent Sources,  Prev: Linear Dependent Sources,  Up: Voltage and Current Sources

8.3.3 Non-linear Dependent Sources
----------------------------------

General form:

          BXXXXXXX N+ N- <I=EXPR> <V=EXPR>

   Examples:

          B1 0 1 I=cos(v(1))+sin(v(2))
          B1 0 1 V=ln(cos(log(v(1,2)^2)))-v(3)^4+v(2)^v(1)
          B1 3 4 I=17
          B1 3 4 V=exp(pi^i(vdd))

   N+ is the positive node, and N- is the negative node.  The values of
the V and I parameters determine the voltages and currents across and
through the device, respectively.  If I is given then the device is a
current source, and if V is given the device is a voltage source.  One
and only one of these parameters must be given.

   The small-signal AC behaviour of the nonlinear source is a linear
dependent source (or sources) with a proportionality constant equal to
the derivative (or derivatives) of the source at the DC operating point.

   The expressions given for V and I may be any function of voltages and
currents through voltage sources in the system.  The following functions
of real variables are defined:

abs            asinh          cosh           sin
acos           atan           exp            sinh
acosh          atanh          ln             sqrt
asin           cos            log            tan

   The function "u" is the unit step function, with a value of one for
arguments greater than zero and a value of zero for arguments less than
zero.  The function "uramp" is the integral of the unit step: for an
input x, the value is zero if x is less than zero, or if x is greater
than zero the value is x. The function "u2" returns a value of zero for
arguments less than zero, one for arguments greater than one and assumes
the value of the argument between these limits .These three functions
are useful in sythesizing piece-wise non-linear functions, though
convergence may be adversely affected.

   Note: "u2" function has been introduced in rework-11.

   The following standard operators are defined:

     +       -       *       /       { }      unary -

   If the argument of log, ln, or sqrt becomes less than zero, the
absolute value of the argument is used.  If a divisor becomes zero or
the argument of log or ln becomes zero, an error will result.  Other
problems may occur when the argument for a function in a partial
derivative enters a region where that function is undefined.

   To get time into the expression you can integrate the current from a
constant current source with a capacitor and use the resulting voltage
(don't forget to set the initial voltage across the capacitor).
Non-linear resistors, capacitors, and inductors may be synthesized with
the nonlinear dependent source.  Non-linear resistors are obvious.
Nonlinear capacitors and inductors are implemented with their linear
counterparts by a change of variables implemented with the nonlinear
dependent source.  The following subcircuit will implement a nonlinear
capacitor:

       .Subckt nlcap   pos neg
       * Bx: calculate f(input voltage)
       Bx   1    0    v = f(v(pos,neg))
       * Cx: linear capacitance
       Cx   2    0    1
       * Vx: Ammeter to measure current into the capacitor
       Vx   2    1    DC 0Volts
       * Drive the current through Cx back into the circuit
       Fx   pos  neg  Vx 1
       .ends

   Non-linear inductors are similar.


File: ngspice.info,  Node: Transmission Lines,  Next: Transistors and Diodes,  Prev: Voltage and Current Sources,  Up: Circuit Elements and Models

8.4 Transmission Lines
======================

* Menu:

* Lossless Transmission Lines::
* Lossy Transmission Lines::
* Lossy Transmission Line Model (LTRA)::
* Uniform Distributed RC Lines (Lossy)::
* Uniform Distributed RC Model (URC)::


File: ngspice.info,  Node: Lossless Transmission Lines,  Next: Lossy Transmission Lines,  Prev: Transmission Lines,  Up: Transmission Lines

8.4.1 Lossless Transmission Lines
---------------------------------

General form:

       TXXXXXXX N1 N2 N3 N4 Z0=VALUE <TD=VALUE> <F=FREQ <NL=NRMLEN>>
       +                    <IC=V1, I1, V2, I2>

   Examples:

       T1 1 0 2 0 Z0=50 TD=10NS

   N1 and N2 are the nodes at port 1; N3 and N4 are the nodes at port 2.
Z0 is the characteristic impedance.  The length of the line may be
expressed in either of two forms.  The transmission delay, TD, may be
specified directly (as TD=10ns, for example).  Alternatively, a
frequency F may be given, together with NL, the normalized electrical
length of the transmission line with respect to the wavelength in the
line at the frequency F.  If a frequency is specified but NL is omitted,
0.25 is assumed (that is, the frequency is assumed to be the
quarter-wave frequency).  Note that although both forms for expressing
the line length are indicated as optional, one of the two must be
specified.

   Note that this element models only one propagating mode.  If all four
nodes are distinct in the actual circuit, then two modes may be excited.
To simulate such a situation, two transmission-line elements are
required.  (see the example in Appendix A for further clarification.)

   The (optional) initial condition specification consists of the
voltage and current at each of the transmission line ports.  Note that
the initial conditions (if any) apply 'only' if the UIC option is
specified on the .TRAN control line.

   Note that a lossy transmission line (see below) with zero loss may be
more accurate than than the lossless transmission line due to
implementation details.


File: ngspice.info,  Node: Lossy Transmission Lines,  Next: Lossy Transmission Line Model (LTRA),  Prev: Lossless Transmission Lines,  Up: Transmission Lines

8.4.2 Lossy Transmission Lines
------------------------------

General form:

       OXXXXXXX N1 N2 N3 N4 MNAME

   Examples:

       O23 1 0 2 0 LOSSYMOD
       OCONNECT 10 5 20 5 INTERCONNECT

   This is a two-port convolution model for singleconductor lossy
transmission lines.  N1 and N2 are the nodes at port 1; N3 and N4 are
the nodes at port 2.  Note that a lossy transmission line with zero loss
may be more accurate than than the lossless transmission line due to
implementation details.


File: ngspice.info,  Node: Lossy Transmission Line Model (LTRA),  Next: Uniform Distributed RC Lines (Lossy),  Prev: Lossy Transmission Lines,  Up: Transmission Lines

8.4.3 Lossy Transmission Line Model (LTRA)
------------------------------------------

The uniform RLC/RC/LC/RG transmission line model (referred to as the
LTRA model henceforth) models a uniform constant-parameter distributed
transmission line.  The RC and LC cases may also be modelled using the
URC and TRA models; however, the newer LTRA model is usually faster and
more accurate than the others.  The operation of the LTRA model is based
on the convolution of the transmission line's impulse responses with its
inputs (see [8]).

   The LTRA model takes a number of parameters, some of which must be
given and some of which are optional.

name        parameter                     units/type     default example
name        parameter                     units/type     default example
R           resistance/length             Z/unit         0.0     0.2
L           inductance/length             henrys/unit    0.0     9.13e-9
G           conductance/length            mhos/unit      0.0     0.0
C           capacitance/length            farads/unit    0.0     3.65e-12
LEN         length of line                no default     1.0     
REL         breakpoint control            arbitrary      1       0.5
                                          unit                   
ABS         breakpoint control            1              5       
NOSTEPLIMIT don't limit timestep to less  flag           not     set
            than line delay                              set     
NOCONTROL   don't do complex timestep     flag           not     set
            control                                      set     
LININTERP   use linear interpolation      flag           not     set
                                                         set     
MIXEDINTERP use linear when quadratic     not set        set     
            seems bad                                            
COMPACTREL  special reltol for history    flag           RELTOL  1.0e-3
            compaction                                           
COMPACTABS  special abstol for history    ABSTOL         1.0e-9  
            compaction                                           
TRUNCNR     use Newton-Raphson method     flag           not     set
            for timestep control                         set     
TRUNCDONTCUTdon't limit timestep to keep  flag           not     set
            impulse-response errors low                  set     

   The following types of lines have been implemented so far: RLC
(uniform transmission line with series loss only), RC (uniform RC
line), LC (lossless transmission line), and RG (distributed series
resistance and parallel conductance only).  Any other combination will
yield erroneous results and should not be tried.  The length LEN of the
line must be specified.

   NOSTEPLIMIT is a flag that will remove the default restriction of
limiting time-steps to less than the line delay in the RLC case.
NOCONTROL is a flag that prevents the default limiting of the time-step
based on convolution error criteria in the RLC and RC cases.  This
speeds up simulation but may in some cases reduce the accuracy of
results.  LININTERP is a flag that, when specified, will use linear
interpolation instead of the default quadratic interpolation for
calculating delayed signals.  MIXEDINTERP is a flag that, when
specified, uses a metric for judging whether quadratic interpolation is
not applicable and if so uses linear interpolation; otherwise it uses
the default quadratic interpolation.  TRUNCDONTCUT is a flag that
removes the default cutting of the time-step to limit errors in the
actual calculation of impulse-response related quantities.  COMPACTREL
and COMPACTABS are quantities that control the compaction of the past
history of values stored for convolution.  Larger values of these lower
accuracy but usually increase simulation speed.  These are to be used
with the TRYTOCOMPACT option, described in the .OPTIONS section.
TRUNCNR is a flag that turns on the use of Newton-Raphson iterations to
determine an appropriate timestep in the timestep control routines. The
default is a trial and error procedure by cutting the previous timestep
in half.  REL and ABS are quantities that control the setting of
breakpoints.

   The option most worth experimenting with for increasing the speed of
simulation is REL.  The default value of 1 is usually safe from the
point of view of accuracy but occasionally increases computation time.
A value greater than 2 eliminates all breakpoints and may be worth
trying depending on the nature of the rest of the circuit, keeping in
mind that it might not be safe from the viewpoint of accuracy.
Breakpoints may usually be entirely eliminated if it is expected the
circuit will not display sharp discontinuities.  Values between 0 and 1
are usually not required but may be used for setting many breakpoints.

   COMPACTREL may also be experimented with when the option
TRYTOCOMPACT is specified in a .OPTIONS card.  The legal range is
between 0 and 1.  Larger values usually decrease the accuracy of the
simulation but in some cases improve speed.  If TRYTOCOMPACT is not
specified on a .OPTIONS card, history compaction is not attempted and
accuracy is high.  NOCONTROL, TRUNCDONTCUT and NOSTEPLIMIT also tend to
increase speed at the expense of accuracy.


File: ngspice.info,  Node: Uniform Distributed RC Lines (Lossy),  Next: Uniform Distributed RC Model (URC),  Prev: Lossy Transmission Line Model (LTRA),  Up: Transmission Lines

8.4.4 Uniform Distributed RC Lines (Lossy)
------------------------------------------

General form:

       UXXXXXXX N1 N2 N3 MNAME L=LEN <N=LUMPS>

   Examples:

       U1 1 2 0 URCMOD L=50U
       URC2 1 12 2 UMODL l=1MIL N=6

   N1 and N2 are the two element nodes the RC line connects, while N3 is
the node to which the capacitances are connected.  MNAME is the model
name, LEN is the length of the RC line in meters.  LUMPS, if specified,
is the number of lumped segments to use in modelling the RC line (see
the model description for the action taken if this parameter is
omitted).


File: ngspice.info,  Node: Uniform Distributed RC Model (URC),  Prev: Uniform Distributed RC Lines (Lossy),  Up: Transmission Lines

8.4.5 Uniform Distributed RC Model (URC)
----------------------------------------

The URC model is derived from a model proposed by L.  Gertzberrg in
1974.  The model is accomplished by a subcircuit type expansion of the
URC line into a network of lumped RC segments with internally generated
nodes.  The RC segments are in a geometric progression, increasing
toward the middle of the URC line, with K as a proportionality
constant.  The number of lumped segments used, if not specified for the
URC line device, is determined by the following formula:

                                            2
                    |     R C        |(K-1)|  |
                          _ _      2
                 log|F        2 J L  |-----|  |
                      max
                    |     L L        |  K  |  |

            N =  ------------------------------
                                  log K

   The URC line is made up strictly of resistor and capacitor segments
unless the ISPERL parameter is given a nonzero value, in which case the
capacitors are replaced with reverse biased diodes with a zero-bias
junction capacitance equivalent to the capacitance replaced, and with a
saturation current of ISPERL amps per meter of transmission line and an
optional series resistance equivalent to RSPERL ohms per meter.

name    parameter                        units   default     example 
K       Propagation Constant             -       2.0         1.2     
FMAX    Maximum Frequency of interest    Hz      1.0G        6.5Meg  
RPERL   Resistance per unit length       Z/m     1000        10      
CPERL   Capacitance per unit length      F/m     1.0e-15     1pF     
ISPERL  Saturation Current per unit      A/m     0           -       
        length                                                       
RSPERL  Diode Resistance per unit length Z/m     0           -       


File: ngspice.info,  Node: Transistors and Diodes,  Prev: Transmission Lines,  Up: Circuit Elements and Models

8.5 Transistors and Diodes
==========================

The area factor used on the diode, BJT, JFET, and MESFET devices
determines the number of equivalent parallel devices of a specified
model.  The affected parameters are marked with an asterisk under the
heading 'area' in the model descriptions below.  Several geometric
factors associated with the channel and the drain and source diffusions
can be specified on the MOSFET device line.

   Two different forms of initial conditions may be specified for some
devices.  The first form is included to improve the dc convergence for
circuits that contain more than one stable state.  If a device is
specified OFF, the dc operating point is determined with the terminal
voltages for that device set to zero.  After convergence is obtained,
the program continues to iterate to obtain the exact value for the
terminal voltages.  If a circuit has more than one dc stable state, the
OFF option can be used to force the solution to correspond to a desired
state.  If a device is specified OFF when in reality the device is
conducting, the program still obtains the correct solution (assuming the
solutions converge) but more iterations are required since the program
must independently converge to two separate solutions.  The .NODESET
control line serves a similar purpose as the OFF option.  The .NODESET
option is easier to apply and is the preferred means to aid convergence.

   The second form of initial conditions are specified for use with the
transient analysis.  These are true 'initial conditions' as opposed to
the convergence aids above.  See the description of the .IC control line
and the .TRAN control line for a detailed explanation of initial
conditions.

* Menu:

* Junction Diodes::
* Diode Model (D)::
* Diode Equations::
* Bipolar Junction Transistors (BJTs)::
* BJT Models (NPN/PNP)::
* Junction Field-Effect Transistors (JFETs)::
* JFET Models (NJF/PJF)::
* MOSFETs::
* MOSFET Models (NMOS/PMOS)::
* MESFETs::
* MESFET Models (NMF/PMF)::


File: ngspice.info,  Node: Junction Diodes,  Next: Diode Model (D),  Prev: Transistors and Diodes,  Up: Transistors and Diodes

8.5.1 Junction Diodes
---------------------

General form:

       DXXXXXXX n+ n- mname <area=val> <m=val> <pj=val> <off> <ic=vd> <temp=val>
       +                    <dtemp=val>

   Examples:

       DBRIDGE 2 10 DIODE1
       DCLMP 3 7 DMOD 3.0 IC=0.2

   The pn junction (diode) implemented in NGSPICE expands the original
spice's implementation. Perimetral effects and high injection level
have been introduced into the original model and temperature dependence
of some parameters has been added.

   `n+' and `n-' are the positive and negative nodes, respectively.
`mname' is the model name, `area' is the area factor, `pj' is the
perimeter factor, and `off' indicates an (optional)starting condition
on the device for dc analysis.  If the area factor is omitted, a value
of 1.0 is assumed. The (optional) initial condition specification using
`ic' is intended for use with the `uic' option on the `.tran' control
line, when a transient analysis is desired starting from other than the
quiescent operating point. You should supply the inital voltage across
the diode there. The (optional) `temp' value is the temperature at
which this device is to operate, and overrides the temperature
specification on the `.option' control line. As always, instance
temperature can be specified as an offset to the circuit temperature
with the `dtemp' option.


File: ngspice.info,  Node: Diode Model (D),  Next: Diode Equations,  Prev: Junction Diodes,  Up: Transistors and Diodes

8.5.2 Diode Model (D)
---------------------

The dc characteristics of the diode are determined by the parameters
`IS' and `N'.  An ohmic resistance, `RS', is included. Charge storage
effects are modelled by a transit time, `TT', and a nonlinear depletion
layer capacitance which is determined by the parameters `CJO', `VJ',
and `M'.  The temperature dependence of the saturation current is
defined by the parameters `EG', the energy and `XTI', the saturation
current temperature exponent. The nominal temperature at which these
parameters were measured is `TNOM', which defaults to the circuit-wide
value specified on the `.options' control line.  Reverse breakdown is
modelled by an exponential increase in the reverse diode current and is
determined by the parameters `BV' and `IBV' (both of which are positive
numbers).

   JUNCTION DC PARAMETERS
name    parameter                     units   default     example     scale
                                                                      factor
BV      reverse breakdown voltage     V       infinite    40.0        
IBV     current at breakdown voltage  A       1.0e-3      1.0e-4      
IK      forward knee current          A       1.0e-3      1.0e-6      
(IKF)                                                                 
IK      reverse knee current          A       1.0e-3      1.0e-6      
IS      saturation current            A       1.0e-14     1.0e-16     area
(JS)                                                                  
JSW     Sidewall saturation current   A       1.0e-14     1.0e-15     perim.
N       emission coefficient          -       1           1.5         
RS      ohmic resistance              Ohm     0           100         1/area

   JUNCTION CAPACITANCE PARAMETERS
name    parameter                     units   default     example     scale
                                                                      factor
CJO     zero-bias junction bottowall  F       0.0         2pF         area
(CJ0)   capacitance                                                   
CJP     zero-bias junction sidewall   F       0.0         .1pF        perim.
(CJSW)  capacitance                                                   
FC      coefficient for forward-bias  -       0.5         -           
        depletion bottomwall                                          
        capacitance formula                                           
FCS     coefficient for forward-bias  -       0.5         -           
        depletion sidewall                                            
        capacitance formula                                           
M (MJ)  Area junction grading         -       0.5         0.5         
        coefficient                                                   
MJSW    Periphery junction grading    -       0.33        0.5         
        coefficient                                                   
VJ      junction potential            V       1           0.6         
PHP     Periphery junction potential  V       1           0.6         
TT      transit-time                  sec     0           0.1ns       

   TEMPERATURE EFFECTS
name    parameter                     units   default     example     scale
                                                                      factor
EG      activation energy             eV      1.11        1.11 Si     
                                                          0.69 Sbd    
                                                          0.67 Ge     
TM1     1st order tempco for MJ       1/^oC   0.0         -           
TM2     2nd order tempco for MJ       1/^oC^2 0.0         -           
TNOM    parameter measurement         C       27          50          
        temperature                                                   
TRS     1st order tempco for RS       1/^oC   0.0         -           
TRS2    2nd order tempco for RS       1/^oC^2 0.0         -           
TTT1    1st order tempco for TT       1/^oC   0.0         -           
TTT2    2nd order tempco for TT       1/^oC^2 0.0         -           
XTI     saturation-current temp. exp  -       3.0         3.0 pn      
                                                          2.0 Sbd     

   NOISE MODELING
name    parameter                     units   default     example     scale
                                                                      factor
KF      flicker noise coefficient     -       0                       
AF      flicker noise exponent        -       1                       


File: ngspice.info,  Node: Diode Equations,  Next: Bipolar Junction Transistors (BJTs),  Prev: Diode Model (D),  Up: Transistors and Diodes

8.5.3 Diode Equations
---------------------

The junction diode is the the basic semiconductor device and the
simplest one modeled in NGSPICE, but it's model is quite complex, even
if not all the physical phenomena affecting a pn junction are modelled.
The diode is modeled in three different regions:

   *      Forward bias: the anode is more positive than the cathode, the
         diode is "on" and can conduct large currents. To avoid
     convergence      problems and unrealistic high current, it is
     better to specify a      series resistance to limit current with
     `RS' model parameter.

   *      Reverse bias: the cathode is more positive than the anode and
         the diode is "off". A reverse bias diode conducts a small
     leakage      current.

   *      Breakdown: the breakdown region is modelled only if the `BV'
        model parameter is given. When a diode enters breakdown the
     current      increase exponentially (remember to limit it). `BV'
     is a      positive value.

   PARAMETERS SCALING

   Model parameters are scaled using the unitless parameters `AREA' and
`PJ' and the multiplier `M' as depicted below:

                    AREAeff = AREA * M
     	       PJeff = PJ * M
                    ISeff = IS * AREAeff + JSW * PJeff
                    IKeff = IK * AREAeff
                    IKReff = IKR * AREAeff
     	       CJeff = CJ0 * AREAeff
     	       CJPeff = CJP * PJeff

   DIODE DC, TRANSIENT AND AC MODEL EQUATIONS

                 To be written!

   The breakdown region must be described with more depth since the
breakdown is not modelled in physically.  As written before, the
breakdown modelling is based on two model parameters: the "nominal
breakdown voltage" `BV' and the current at the onset of breakdown
`IBV'. For the diode model to be consistent, the current value cannot
be arbitrary chosen, since the reverse bias and breakdown regions must
match.

   When the diode enters breakdown region from reverse bias, the current
is calculated using the formula:

                 To be written!

   NOTE: if you look at the code in `diotemp.c' you will discover that
the exponential relation is replaced with a first order taylor series
expansion.

   The computed current is necessary to adjust the breakdown voltage
making the two regions match. The algorithm is a little bit convoluted
and only a brief description is given here:


     IF IBVeff < Ibdwm THEN
        IBVeff = Ibwn
        BVeff = BV
     ELSE
        BVeff = BV - N * Vt * LN(IBVeff/Ibdvn)
     END IF

   Most real diodes shows a current increase that, at high current
levels, does not follow the exponential relationship given above. This
behaviour is due to high level of carriers injected into the junction.
High injection effects (as they are called) are modelled with `IK' and
`IKR'.


                 Not yet written!

   Diode capacitance is divided into two different terms:

   * Depletion capacitance

   * Diffusion capacitance

   Depletion capacitance is composed by two different contributes, one
associated to the bottom of the junction (bottowall depletion
capacitance) and the other to the periphery (sidewall depletion
capacitance).

   The basic equations are:


            Cdiode = Cdiffusion + Cdepletion

   Where the depletion capacitance i defined as:


            Cdepletion = CdeplBW + CdeplSW

   The diffusion capacitance, due to the injected minority carriers is
modeled with the transit time `TT':


                           dIDeff
              Cdiffusion = ----- * TT
                            dVd

   The depletion capacitance is more complex to model, since the
function used to approximate it diverges when the diode voltage become
greater than the junction built-in potential. To avoid function
divergence, the capacitance function is approximated with a linear
extrapolation for applied voltage greater than a fraction of the
junction built-in potential.


                 Not yet written!

   The temperature affects many of the parameters in the equations
above, the following equations show how. One of the most significant
parameter that varies with the temperature for a semiconductor is the
band-gap energy:

                                                2
     				       TNOM
             EGnom = 1.16 - 7.02e-4 * ---------------
                                       TNOM + 1108.0

     	                                 2
     	                                T
     	EG(T) = 1.16 - 7.02e-4 * ---------------
     			          TNOM + 1108.0

   The leakeage currents temperature dependence is:

                                   logfactor
     			      ---------
                                       N
                   IS(T)  =  IS * e

     	                      logfactor
     	                      ---------
     	                          N
     	      JSW(T) = JSW * e

   where "logfactor" is defined:

                            EG        EG                T
             logfactor = -------- - ----- + XTI * ln ( ---- )
                         Vt(TNOM)   Vt(t)              TNOM

   The contact potentials (bottowall an sidewall) temperature
dependence is:

                            T                            T        EGnom     EG(T)
           VJ(T) = VJ * ( ----- ) - Vt(T) * [ 3 * ln ( ----- ) + -------- - ----- ]
                          TNOM                         TNOM      Vt(TNOM)   Vt(T)


                              T                            T        EGnom     EG(T)
           PHP(T) = PHP * ( ----- ) - Vt(T) * [ 3 * ln ( ----- ) + -------- - ----- ]
                            TNOM                         TNOM      Vt(TNOM)   Vt(T)

   The depletion capacitances temperature dependence is:

                                                         PB(T)
           CJ(T) = CJ * [1 + MJ * (4.0e-4 * (T - TMON) - ----- + 1) ]
                                                           PB

                                                             PHP(T)
           CJSW(T) = CJSW * [1 + MJ * (4.0e-4 * (T - TMON) - ------ + 1) ]
                                                              PHP

   The transit time temperature dependence is:

           TT(T) = TT * (1 + TTT1 * (T - TNOM) + TTT2) * (T -TNOM)^2)

   The junction grading coefficient temperature dependence is:

           MJ(T) = MJ * (1 + TM1 * (T - TNOM) + TM2) * (T -TNOM)^2)

   The series resistance temperature dependence is:

           RS(T) = RS * (1 + TRS * (T - TNOM) + TRS2) * (T -TNOM)^2)


File: ngspice.info,  Node: Bipolar Junction Transistors (BJTs),  Next: BJT Models (NPN/PNP),  Prev: Diode Equations,  Up: Transistors and Diodes

8.5.4 Bipolar Junction Transistors (BJTs)
-----------------------------------------

General form:

       QXXXXXXX nc nb ne <ns> mname <area=val> <areac=val> <areab=val>
       + <m=val> <off> <ic=vbe, vce> <temp=val> <dtemp=val>

   Examples:

       Q23 10 24 13 QMOD IC=0.6, 5.0
       Q50A 11 26 4 20 MOD1

   `nc', `nb', and `ne' are the collector, base, and emitter nodes,
respectively. `ns' is the (optional) substrate node.If unspecified,
ground is used.  `mname' is the model name, `area', `areab', `areac'
are the area factors, and `off' indicates an (optional) initial
condition on the device for the dc analysis.  If the area factor is
omitted, a value of 1.0 is assumed.  The (optional) initial condition
specification using `ic=vbe, vce' is intended for use with the  `uic'
`.tran' control line, when a transient analysis is desired starting
from other than the quiescent operating point.  See the `.ic' control
line description for a better way to set transient initial conditions.
The (optional) `temp' value is the temperature at which this device is
to operate, and overrides the temperature specification on the
`.option' control line. Using `dtemp' option you can specify instance's
temperature relative to the circuit temperature.


File: ngspice.info,  Node: BJT Models (NPN/PNP),  Next: Junction Field-Effect Transistors (JFETs),  Prev: Bipolar Junction Transistors (BJTs),  Up: Transistors and Diodes

8.5.5 BJT Models (NPN/PNP)
--------------------------

NGSPICE provides two BJT device models. The `level' specifies the model
to be used:

   * level=1 : This is the original spice BJT model, and it is the
               default model if the `level' keyword is not
     specified on the `.model' line.

   * level=2 : This is a modified version of the original spice
            BJT that models both vertical and lateral devices and
     includes temperature corrections of collector, 		emitter and base
     resistors.

   The bipolar junction transistor model in NGSPICE is an adaptation of
the integral charge control model of Gummel and Poon.  This modified
Gummel-Poon model extends the original model to include several effects
at high bias levels.  The model automatically simplifies to the simpler
Ebers-Moll model when certain parameters are not specified.  The
parameter names used in the modified Gummel-Poon model have been chosen
to be more easily understood by the program user, and to reflect better
both physical and circuit design thinking.

   The dc model is defined by the parameters `IS', `BF', `NF', `ISE',
`IKF', amd `NE' which determine the forward current gain
characteristics, `IS', `BR', `NR', `ISC', `IKR', and `NC' which
determine the reverse current gain characteristics, and `VAF' and `VAR'
which determine the output conductance for forward and reverse regions.
Level 2 model includes substrate saturation current `ISS'.

   Three ohmic resistances `RB', `RC', and `RE' are included, where
`RB' can be high current dependent.  Base charge storage is modelled by
forward and reverse transit times, `TF' and `TR', the forward transit
time `TF' being bias dependent if desired, and nonlinear depletion
layer capacitances which are determined by `CJE', `VJE', and `NJE' for
the B-E junction, `CJC', `VJC', and `NJC' for the B-C junction and
`CJS', `VJS', and `MJS' for the C-S (Collector-Substrate) junction.
Level 2 model defines a substrate capacitance that will be connected to
device's base or collector, to model lateral or vertical devices.

   The temperature dependence of the saturation currents, `IS' and
`ISS' (for level 2 model), is determined by the energy-gap, `EG', and
the saturation current temperature exponent, `XTI'.  Additionally base
current temperature dependence is modelled by the beta temperature
exponent `XTB' in the new model.  The values specified are assumed to
have been measured at the temperature `TNOM', which can be specified on
the `.options' control line or overridden by a specification on the
`.model' line.

   The BJT parameters used in the modified Gummel-Poon model are listed
below.  The parameter names used in earlier versions of SPICE2 are still
accepted.

   Modified Gummel-Poon BJT Parameters:

name    parameter                     units   default     example     scale
                                                                      factor
SUBS    substrate connection: 1 for   1                   1.0e-15     
                        vertical                                      
        geometry, -1 for 		  lateral                                  
        geometry.  		  (level                                         
        2 only)                                                       
IS      transport saturation current  A       1.0e-16     1.0e-15     area
ISS     reverse saturation current,   A       1.0e-16     1.0e-15     area
        substrate-to-collector for                                    
            vertical device or                                        
            substrate-to-base for                                     
        lateral 	     (level                                          
        2 only)                                                       
BF      ideal maximum forward beta    -       100         100         
NF      forward current emission      -       1.0         1           
                     coefficient                                      
VAF     forward Early voltage         V       infinite    200         
IKF     corner for forward beta       A       infinite    0.01        area
                    current                                           
        roll-off                                                      
ISE     B-E leakage saturation        A       0           1.0e-13     area
        current                                                       
NE      B-E leakage emission          -       1.5         2           
        coefficient                                                   
BR      ideal maximum reverse beta    -       1           0.1         
NR      reverse current emission      -       1           1           
        coefficient                                                   
VAR     reverse Early voltage         V       infinite    200         
IKR     corner for reverse beta high  A       infinite    0.01        area
        current roll-off                                              
ISC     B-C leakage saturation        A       0           1.0e-13     area
        current                                                       
        (area is "areab" for vertical                                 
          devices and "areac" for                                     
        lateral)                                                      
NC      B-C leakage emission          -       2           1.5         
        coefficient                                                   
RB      zero bias base resistance     Z       0           100         area
IRB     current where base            A       infinite    0.1         area
               resistance falls                                       
        halfway 		  to its min                                        
        value                                                         
RBM     minimum base resistance at    Z       RB 10       area        
        high currents                                                 
RE      emitter resistance            Z       0           1           area
RC      collector resistance          Z       0           10          area
CJE     B-E zero-bias depletion       F       0           2pF         area
        capacitance                                                   
VJE     B-E built-in potential        V       0.75        0.6         
MJE     B-E junction exponential      -       0.33        0.33        
        factor                                                        
TF      ideal forward transit time    sec     0           0.1ns       
XTF     coefficient for bias          -       0                       
        dependence of TF                                              
VTF     voltage describing VBC        V       infinite                
        dependence of TF                                              
ITF     high-current parameter for    A       0           -           area
        effect on TF                                                  
PTF     excess phase at               deg     0                       
        freq=1.0/(TF*2PI) Hz                                          
CJC     B-C zero-bias depletion       F       0           2pF         area
        capacitance                                                   
        (area is "areab" for                                          
        vertical 		   devices                                         
        and "areac" for lateral)                                      
VJC     B-C built-in potential        V       0.75        0.5         
MJC     B-C junction exponential      -       0.33        0.5         
        factor                                                        
XCJC    fraction of B-C depletion     -       1                       
        capacitance connected to                                      
        internal base node                                            
TR      ideal reverse transit time    sec     0           10ns        
CJS     zero-bias                     F       0           2pF         area
        collector-substrate                                           
        capacitance                                                   
        (area is "areac" for                                          
        vertical devices and                                          
        "areab" for lateral)                                          
VJS     substrate junction built-in   V       0.75                    
        potential                                                     
MJS     substrate junction            -       0           0.5         
        exponential factor                                            
XTB     forward and reverse beta      -        0                      
        temperature exponent                                          
EG      energy gap for temperature    eV      1.11                    
        effect on IS                                                  
XTI     temperature exponent for      -       3                       
        effect on IS                                                  
KF      flicker-noise coefficient     -       0                       
AF      flicker-noise exponent        -       1                       
FC      coefficient for forward-bias  -       0.5         o           
        depletion capacitance formula                                 
TNOM    Parameter measurement         ^oC     27          50          
        temperature                                                   
TRE1    1st order temperature         1/^oC   0.0         1e-3        
        coefficient for RE                                            
               (level 2 only)                                         
TRE2    2nd order temperature         1/^oC^2 0.0         1e-5        
        coefficient for RE                                            
               (level 2 only)                                         
TRC1    1st order temperature         1/^oC   0.0         1e-3        
        coefficient for RC                                            
               (level 2 only )                                        
TRC2    2nd order temperature         1/^oC^2 0.0         1e-5        
        coefficient for RC                                            
               (level 2 only)                                         
TRB1    1st order temperature         1/^oC   0.0         1e-3        
        coefficient for RB                                            
               (level 2 only)                                         
TRB2    2nd order temperature         1/^oC^2 0.0         1e-5        
        coefficient for RB                                            
               (level 2 only)                                         
TRB1    1st order temperature         1/^oC   TRB1        1e-3        
        coefficient for RBM                                           
                (level 2 only)                                        
TRB2    2nd order temperature         1/^oC^2 TRB2        1e-5        
        coefficient for RBM                                           
                (level 2 only)                                        


File: ngspice.info,  Node: Junction Field-Effect Transistors (JFETs),  Next: JFET Models (NJF/PJF),  Prev: BJT Models (NPN/PNP),  Up: Transistors and Diodes

8.5.6 Junction Field-Effect Transistors (JFETs)
-----------------------------------------------

General form:

       JXXXXXXX ND NG NS MNAME <AREA> <OFF> <IC=VDS, VGS> <TEMP=T>

   Examples:

       J1 7 2 3 JM1 OFF

   ND, NG, and NS are the drain, gate, and source nodes, respectively.
MNAME is the model name, AREA is the area factor, and OFF indicates an
(optional) initial condition on the device for dc analysis.  If the area
factor is omitted, a value of 1.0 is assumed.  The (optional) initial
condition specification, using IC=VDS, VGS is intended for use with the
UIC option on the .TRAN control line, when a transient analysis is
desired starting from other than the quiescent operating point.  See the
.IC control line for a better way to set initial conditions.  The
(optional) TEMP value is the temperature at which this device is to
operate, and overrides the temperature specification on the .OPTION
control line.


File: ngspice.info,  Node: JFET Models (NJF/PJF),  Next: MOSFETs,  Prev: Junction Field-Effect Transistors (JFETs),  Up: Transistors and Diodes

8.5.7 JFET Models (NJF/PJF)
---------------------------

The JFET model is derived from the FET model of Shichman and Hodges.
The dc characteristics are defined by the parameters VTO and BETA, which
determine the variation of drain current with gate voltage, LAMBDA,
which determines the output conductance, and IS, the saturation current
of the two gate junctions.  Two ohmic resistances, RD and RS, are
included.  Charge storage is modelled by nonlinear depletion layer
capacitances for both gate junctions which vary as the -1/2 power of
junction voltage and are defined by the parameters CGS, CGD, and PB.

   Note that in Spice3f and later, a fitting parameter B has been added.
For details, see [9].

name    parameter                        units       default     example     area
VTO     threshold voltage (V_T0)         V           -2.0        -2.0        
BETA    transconductance parameter (B)   A/V^2       1.0e-4      1.0e-3      *
LAMBDA  channel-length modulation        1/V         0           1.0e-4      
        parameter (L)                                                        
RD      drain ohmic resistance           Z           0           100         *
RS      source ohmic resistance          Z           0           100         *
CGS     zero-bias G-S junction           F           0           5pF         *
        capacitance (C_gs)                                                   
CGD     zero-bias G-D junction           F           0           1pF         *
        capacitance (C_gs)                                                   
PB      gate junction potential          V           1           0.6         
IS      gate junction saturation         A           1.0e-14     1.0e-14     *
        current (I_S)                                                        
B       doping tail parameter            -           1           1.1         
KF      flicker noise coefficient        -           0                       
AF      flicker noise exponent           -           1                       
FC      coefficient for forward-bias     -           0.5                     
        depletion capacitance formula                                        
TNOM    parameter measurement            ^oC         27          50          
        temperature                                                          


File: ngspice.info,  Node: MOSFETs,  Next: MOSFET Models (NMOS/PMOS),  Prev: JFET Models (NJF/PJF),  Up: Transistors and Diodes

8.5.8 MOSFETs
-------------

General form:

       MXXXXXXX ND NG NS NB MNAME <M=VAL> <L=VAL> <W=VAL> <AD=VAL> <AS=VAL>
       + <PD=VAL> <PS=VAL> <NRD=VAL> <NRS=VAL> <OFF>
       + <IC=VDS, VGS, VBS> <TEMP=T>

   Examples:

       M1 24 2 0 20 TYPE1
       M31 2 17 6 10 MODM L=5U W=2U
       M1 2 9 3 0 MOD1 L=10U W=5U AD=100P AS=100P PD=40U PS=40U

   ND, NG, NS, and NB are the drain, gate, source, and bulk (substrate)
nodes, respectively.  MNAME is the model name. M is the multiplicity
parameter, which simulates m paralleled devices. All MOS models support
the "M" parameter. L and W are the channel length and width, in meters.
AD and AS are the areas of the drain and source diffusions, in
meters^2.

   Note that the suffix U specifies microns (1e-6 m) and P sq-microns
(1e-12 m^2). If any of L, W, AD, or AS are not specified, default
values are used.  The use of defaults simplifies input file
preparation, as well as the editing required if device geometries are
to be changed.  PD and PS are the perimeters of the drain and source
junctions, in meters.  NRD and NRS designate the equivalent number of
squares of the drain and source diffusions; these values multiply the
sheet resistance RSH specified on the .MODEL control line for an
accurate representation of the parasitic series drain and source
resistance of each transistor.  PD and PS default to 0.0 while NRD and
NRS to 1.0.  OFF indicates an (optional) initial condition on the
device for dc analysis.  The (optional) initial condition specification
using IC=VDS, VGS, VBS is intended for use with the UIC option on the
.TRAN control line, when a transient analysis is desired starting from
other than the quiescent operating point.  See the .IC control line for
a better and more convenient way to specify transient initial
conditions.  The (optional) TEMP value is the temperature at which this
device is to operate, and overrides the temperature specification on
the .OPTION control line.  The temperature specification is ONLY valid
for level 1, 2, 3, and 6 MOSFETs, not for level 4 or 5 (BSIM) devices.


File: ngspice.info,  Node: MOSFET Models (NMOS/PMOS),  Next: MESFETs,  Prev: MOSFETs,  Up: Transistors and Diodes

8.5.9 MOSFET Models (NMOS/PMOS)
-------------------------------

MOSFET models are the central part of NGSPICE, probably because they are
the most widely used devices in the electronics world. NGSPICE provides
all the MOSFETs implemented in the original Spice3f and adds several
models developed by Berkeley's Device Group and other independent
groups. Not all models below are included in the standard NGSPICE
distribution because of copyright restrictions.

   NGSPICE provides four MOSFET device models, which differ in the
formulation of the I-V characteristic.  The variable LEVEL specifies the
model to be used:

LEVEL   Model                    Notes
1       Shichman-Hodges          The classical model
2       MOS2                     Described in [2]
3       MOS3                     A semi-empirical model (see [1])
4       BSIM                     Described in [3]
5       BSIM2                    Described in [5]
6       MOS6                     Described in [2]
8       BSIM3                    Described in [13]
9       MOS9                     n/a
10      B3SOI                    n/a
14      BSIM4                    n/a
17      HiSIM1                   n/a
29      B3SOIPD                  n/a
30      B3SOIFD                  n/a
31      B3SOIDD                  n/a
14      BSIM4                    n/a
44      EKV                      n/a
49      BSIM3v1s                 n/a (Serban Version)
50      BSIM3v1                  n/a (Berkeley Version)
51      BSIM3v1a                 n/a (Alan Version)
52      BSIM3v0                  n/a (Berkeley Version)
62      STAG                     n/a

   Level 44 model (EKV) is not available in the standard distribution
since it is not released in source form. To obtain the code please
refer to the EKV group home page (http://legwww.epfl.ch/ekv/).

   The dc characteristics of the level 1 through level 3 MOSFETs are
defined by the device parameters VTO, KP, LAMBDA, PHI and GAMMA.  These
parameters are computed by NGSPICE if process parameters (NSUB, TOX,
...)  are given, but users specified values always override.  VTO is
positive (negative) for enhancement mode and negative (positive) for
depletion mode N-channel (P-channel) devices.  Charge storage is
modelled by three constant capacitors, CGSO, CGDO, and CGBO which
represent overlap capacitances, by the nonlinear thin-oxide capacitance
which is distributed among the gate, source, drain, and bulk regions,
and by the nonlinear depletion-layer capacitances for both substrate
junctions divided into bottom and periphery, which vary as the MJ and
MJSW power of junction voltage respectively, and are determined by the
parameters CBD, CBS, CJ, CJSW, MJ, MJSW and PB.  Charge storage effects
are modelled by the piecewise linear voltages-dependent capacitance
model proposed by Meyer.  The thin-oxide charge-storage effects are
treated slightly different for the LEVEL=1 model.  These
voltage-dependent capacitances are included only if TOX is specified in
the input description and they are represented using Meyer's
formulation.

   There is some overlap among the parameters describing the junctions,
e.g. the reverse current can be input either as IS (in A) or as JS (in
A/m^2). Whereas the first is an absolute value the second is multiplied
by AD and AS to give the reverse current of the drain and source
junctions respectively.  This methodology has been chosen since there
is no sense in relating always junction characteristics with AD and AS
entered on the device line; the areas can be defaulted.  The same idea
applies also to the zero-bias junction capacitances CBD and CBS (in F)
on one hand, and CJ (in F/m^2) on the other.  The parasitic drain and
source series resistance can be expressed as either RD and RS (in ohms)
or RSH (in ohms/sq.), the latter being multiplied by the number of
squares NRD and NRS input on the device line.

   A discontinuity in the MOS level 3 model with respect to the KAPPA
parameter has been detected (see [10]).  The supplied fix has been
implemented in Spice3f2 and later.  Since this fix may affect parameter
fitting, the option "BADMOS3" may be set to use the old implementation
(see the section on simulation variables and the ".OPTIONS" line).
NGSPICE level 1, 2, 3 and 6 parameters:

name    parameter                        units       default     example
LEVEL   model index                      -           1           
VTO     zero-bias threshold voltage      V           0.0         1.0
        (V_T0)                                                   
KP      transconductance parameter       A/V^2       2.0e-5      3.1e-5
GAMMA   bulk threshold parameter         V^1/2       0.0         0.37
PHI     surface potential (U)            V           0.6         0.65
LAMBDA  channel-length modulation (MOS1  1/V         0.0         0.02
        and MOS2 only) (L)                                       
RD      drain ohmic resistance           Z           0.0         1.0
RS      source ohmic resistance          Z           0.0         1.0
CBD     zero-bias B-D junction           F           0.0         20fF
        capacitance                                              
CBS     zero-bias B-S junction           F           0.0         20fF
        capacitance                                              
IS      bulk junction saturation         A           1.0e-14     1.0e-15
        current (I_S)                                            
PB      bulk junction potential          V           0.8         0.87
CGSO    gate-source overlap capacitance  F/m         0.0         4.0e-11
        per meter channel width                                  
CGDO    gate-drain overlap capacitance   F/m         0.0         4.0e-11
        per meter channel width                                  
CGBO    gate-bulk overlap capacitance    F/m         0.0         2.0e-10
        per meter channel length                                 
RSH     drain and source diffusion       Z/[]        0.0         10.0
        sheet resistance                                         
CJ      zero-bias bulk junction bottom   F/m^2       0.0         2.0e-4
        cap. per sq-meter of junction                            
        area                                                     
MJ      bulk junction bottom grading     -           0.5         0.5
        coeff.                                                   
CJSW    zero-bias bulk junction          F/m         0.0         1.0e-9
        sidewall cap. per meter of                               
        junction perimeter                                       
MJSW    bulk junction sidewall grading   -           0.50(level1),
        coeff.                                       0.33(level2,
                                                     3)          
JS      bulk junction saturation         A/m^2       1.0e-8      
        current per sq-meter of                                  
        junction area                                            
TOX     oxide thickness                  meter       1.0e-7      1.0e-7
NSUB    substrate doping                 1/cm^3      0.0         4.0e15
NSS     surface state density            1/cm^2      0.0         1.0e10
NFS     fast surface state density       1/cm^2      0.0         1.0e10
TPG     type of gate material:           -           1.0         
              +1 opp. to substrate, -1                           
        same as substrate, 0  Al gate                            
XJ      metallurgical junction depth     meter       0.0         1M
LD      lateral diffusion                meter       0.0         0.8M
UO      surface mobility                 cm^2/Vs     600         700
UCRIT   critical field for mobility      V/cm        1.0e4       1.0e4
        degradation (MOS2 only)                                  
UEXP    critical field exponent in       -           0.0         0.1
        mobility degradation (MOS2 only)                         
UTRA    transverse field coeff.          -           0.0         0.3
        (mobility) (deleted for MOS2)                            
VMAX    maximum drift velocity of        m/s         0.0         5.0e4
        carriers                                                 
NEFF    total channel-charge (fixed and  -           1.0         5.0
        mobile) coefficient (MOS2 only)                          
KF      flicker noise coefficient        -           0.0         1.0e-26
AF      flicker noise exponent           -           1.0         1.2
FC      coefficient for forward-bias     -           0.5         
        depletion capacitance formula                            
DELTA   width effect on threshold        -           0.0         1.0
        voltage (MOS2 and MOS3)                                  
THETA   mobility modulation (MOS3 only)  1/V         0.0         0.1
ETA     static feedback (MOS3 only)      -           0.0         1.0
KAPPA   saturation field factor (MOS3    -           0.2         0.5
        only)                                                    
TNOM    parameter measurement            ^oC         27          50
        temperature                                              

   The level 3 model available into ngspice takes into account length
and width mask adjustments (`xl' and `xw') and device width narrowing
due to diffusion (`wd').

   The level 4 and level 5 (BSIM1 and BSIM2) parameters are all values
obtained from process characterization, and can be generated
automatically.  J. Pierret [4] describes a means of generating a
'process' file, and the program Proc2Mod provided with NGSPICE converts
this file into a sequence of BSIM1 ".MODEL" lines suitable for inclusion
in a NGSPICE input file.  Parameters marked below with an * in the l/w
column also have corresponding parameters with a length and width
dependency.  For example, VFB is the basic parameter with units of
Volts, and LVFB and WVFB also exist and have units of Volt-Mmeter The
formula

                           P            P
                            L            W
              P = P  + ---------- + ----------
                   0
                       L            W
                        effective    effective

   is used to evaluate the parameter for the actual device specified
with

                  L          = L      - DL
                   effective    input

   and

                  W          = W      - DW
                   effective    input

   Note that unlike the other models in NGSPICE, the BSIM model is
designed for use with a process characterization system that provides
all the parameters, thus there are no defaults for the parameters, and
leaving one out is considered an error.  For an example set of
parameters and the format of a process file, see the SPICE2
implementation notes[3].

   For more information on BSIM2, see reference [5].

   NGSPICE BSIM (level 4) parameters.

name        parameter                                units          l/w
VFB         flat-band voltage                        V              *
PHI         surface inversion potential              V              *
K1          body effect coefficient                  V^(1/2)        *
K2          drain/source depletion charge-sharing    -              *
            coefficient                                             
ETA         zero-bias drain-induced                  -              *
            barrier-lowering coefficient                            
MUZ         zero-bias mobility                       cm^2/V-s       
DL          shortening of channel                    Mm             
DW          narrowing of channel                     Mm             
U0          zero-bias transverse-field mobility      V^-1           *
            degradation                                             
            coefficient                                             
U1          zero-bias velocity saturation            Mm/V           *
            coefficient                                             
X2MZ        sens. of mobility to substrate bias at   cm^2/V-s       *
            V_ds=0                                                  
X2E         sens. of drain-induced barrier lowering  V^-1           *
            effect to                   substrate                   
            bias                                                    
X3E         sens. of drain-induced barrier lowering  V^-1           *
            effect to                   drain bias                  
            at V_ds=V_dd                                            
X2U0        sens. of transverse field mobility       V^2            *
            degradation                   effect to                 
            substrate bias                                          
X2U1        sens. of velocity saturation effect to   MmV^2          *
            substrate                   bias                        
MUS         mobility at zero substrate bias and at   cm^2/V^2-s     
            V_ds=V_dd                                               
X2MS        sens. of mobility to substrate bias at   cm^2/V^2-s     *
            V_ds=V_dd                                               
X3MS        sens. of mobility to drain bias at       cm^2/V^2-s     *
            V_ds=V_dd                                               
X3U1        sens. of velocity saturation effect on   MmV^2          *
            drain bias                   at                         
            V_ds=V_dd                                               
TOX         gate oxide thickness                     Mm             
TEMP        temperature at which parameters were     C              
            measured                                                
VDD         measurement bias range                   V              
CGDO        gate-drain overlap capacitance per       F/m            
            meter channel                   width                   
CGSO        gate-source overlap capacitance per      F/m            
            meter channel                   width                   
CGBO        gate-bulk overlap capacitance per meter  F/m            
            channel                   length                        
XPART       gate-oxide capacitance-charge model      -              
            flag                                                    
N0          zero-bias subthreshold slope             -              *
            coefficient                                             
NB          sens. of subthreshold slope to           -              *
            substrate bias                                          
ND          sens. of subthreshold slope to drain     -              *
            bias                                                    
RSH         drain and source diffusion sheet         Z/[]           
            resistance                                              
JS          source drain junction current density    A/m^2          
PB          built in potential of source drain       V              
            junction                                                
MJ          Grading coefficient of source drain      -              
            junction                                                
BSW         built in potential of source, drain      V              
            junction                   sidewall                     
MJSW        grading coefficient of source drain      -              
            junction                   sidewall                     
CJ          Source drain junction capacitance per    F/m^2          
            unit area                                               
CJSW        source drain junction sidewall           F/m            
            capacitance per                   unit                  
            length                                                  
WDF         source drain junction default width      m              
DELL        Source drain junction length reduction   m              

   XPART = 0 selects a 40/60 drain/source charge partition in
saturation, while XPART=1 selects a 0/100 drain/source charge partition.

   ND, NG, and NS are the drain, gate, and source nodes, respectively.
MNAME is the model name, AREA is the area factor, and OFF indicates an
(optional) initial condition on the device for dc analysis.  If the area
factor is omitted, a value of 1.0 is assumed.  The (optional) initial
condition specification, using IC=VDS, VGS is intended for use with the
UIC option on the .TRAN control line, when a transient analysis is
desired starting from other than the quiescent operating point.  See the
.IC control line for a better way to set initial conditions.


File: ngspice.info,  Node: MESFETs,  Next: MESFET Models (NMF/PMF),  Prev: MOSFET Models (NMOS/PMOS),  Up: Transistors and Diodes

8.5.10 MESFETs
--------------

General form:

       ZXXXXXXX ND NG NS MNAME <AREA> <OFF> <IC=VDS, VGS>

   Examples:

       Z1 7 2 3 ZM1 OFF


File: ngspice.info,  Node: MESFET Models (NMF/PMF),  Prev: MESFETs,  Up: Transistors and Diodes

8.5.11 MESFET Models (NMF/PMF)
------------------------------

The MESFET model is derived from the GaAs FET model of Statz et al.  as
described in [11].  The dc characteristics are defined by the parameters
VTO, B, and BETA, which determine the variation of drain current with
gate voltage, ALPHA, which determines saturation voltage, and LAMBDA,
which determines the output conductance.  The formula are given by:

                                        3
                       2
             B (V  -V )    |    |   V  |  |                             3
                 gs  T               ds                                 _
      I  = --------------- |1 - |1-A---|  |(1 + L V  )   for  0 < V   <
       d                                           ds              ds
           1 + b(V   - V ) |    |    3 |  |                             A
                  gs    T
                         2
               B (V  -V )                                     3
                   gs  T                                      _
        I  = ---------------(1 + L V  )            for  V   >
         d                          ds                   ds
             1 + b(V   - V )                                  A
                    gs    T

   Two ohmic resistances, RD and RS, are included.  Charge storage is
modeled by total gate charge as a function of gate-drain and gate-source
voltages and is defined by the parameters CGS, CGD, and PB.

name     parameter                             units   default   example   area
VTO      pinch-off voltage                     V       -2.0      -2.0      
BETA     transconductance parameter            A/V^2   1.0e-4    1.0e-3    *
B        doping tail extending parameter       1/V     0.3       0.3       *
ALPHA    saturation voltage parameter          1/V     2         2         *
LAMBDA   channel-length modulation parameter   1/V     0         1.0e-4    
RD       drain ohmic resistance                Z       0         100       *
RS       source ohmic resistance               Z       0         100       *
CGS      zero-bias G-S junction capacitance    F       0         5pF       *
CGD      zero-bias G-D junction capacitance    F       0         1pF       *
PB       gate junction potential               V       1         0.6       
KF       flicker noise coefficient             -       0                   
AF       flicker noise exponent                -       1                   
FC       coefficient for forward-bias          -       0.5                 
                  depletion capacitance                                    
         formula                                                           


File: ngspice.info,  Node: Analyses and Output Control,  Next: Interactive Interpreter,  Prev: Circuit Elements and Models,  Up: Top

9 Analyses and Output Control
*****************************

The following command lines are for specifying analyses or plots within
the circuit description file.  Parallel commands exist in the
interactive command interpreter (detailed in the following section).
Specifying analyses and plots (or tables) in the input file is useful
for batch runs.  Batch mode is entered when either the -b option is
given or when the default input source is redirected from a file.  In
batch mode, the analyses specified by the control lines in the input
file (e.g. ".ac", ".tran", etc.)  are immediately executed (unless
".control" lines exists; see the section on the interactive command
interpreter).  If the -r rawfile option is given then all data generated
is written to a Ngspice rawfile.  The rawfile may be read by either the
interactive mode of Ngspice or by nutmeg; see the previous section for
details.  In this case, the .SAVE line (see below) may be used to record
the value of internal device variables (see Appendix B).

   If a rawfile is not specified, then output plots (in "line-printer"
form) and tables can be printed according to the .PRINT, .PLOT, and
.FOUR control lines, described next.  .PLOT, .PRINT, and .FOUR lines are
meant for compatibility with Spice2.

* Menu:

* Simulator Variables (.OPTIONS)::
* Initial Conditions::
* Analyses::
* Batch Output::


File: ngspice.info,  Node: Simulator Variables (.OPTIONS),  Next: Initial Conditions,  Prev: Analyses and Output Control,  Up: Analyses and Output Control

9.1 Simulator Variables (.OPTIONS)
==================================

Various parameters of the simulations available in Ngspice can be
altered to control the accuracy, speed, or default values for some
devices.  These parameters may be changed via the "set" command
(described later in the section on the interactive front-end) or via
the ".OPTIONS" line:

   General form:

          .OPTIONS OPT1 OPT2 ... (or OPT=OPTVAL ...)

   Examples:

          .OPTIONS RELTOL=.005 TRTOL=8

   The options line allows the user to reset program control and user
options for specific simulation purposes.  Additional options for Nutmeg
may be specified as well and take effect when Nutmeg reads the input
file.  Options specified to Nutmeg via the 'set' command are also passed
on to NGSPICE as if specified on a .OPTIONS line.  See the following
section on the interactive command interpreter for the parameters which
may be set with a .OPTIONS line and the format of the 'set' command.
Any combination of the following options may be included, in any order.
'x' (below) represents some positive number.

`ABSTOL=x'
     resets the absolute current error tolerance of the program.  The
     default value is 1 picoamp.

`BADMOS3'
     Use the older version of the MOS3 model with the "kappa"
     discontinuity.

`CHGTOL=x'
     resets the charge tolerance of the program.  The default value is
     1.0e-14.

`DEFAD=x'
     resets the value for MOS drain diffusion area; the default is 0.0.

`DEFAS=x'
     resets the value for MOS source diffusion area; the default is 0.0.

`DEFL=x'
     resets the value for MOS channel length; the default is 100.0
     micrometer.

`DEFW=x'
     resets the value for MOS channel width; the default is 100.0
     micrometer.

`GMIN=x'
     resets the value of GMIN, the minimum conductance allowed by the
     program.  The default value is 1.0e-12.

`ITL1=x'
     resets the dc iteration limit.  The default is 100.

`ITL2=x'
     resets the dc transfer curve iteration limit.  The default is 50.

`ITL3=x'
     resets the lower transient analysis iteration limit.  the default
     value is 4.  (Note: not implemented in Ngspice).

`ITL4=x'
     resets the transient analysis timepoint iteration limit.  the
     default is 10.

`ITL5=x'
     resets the transient analysis total iteration limit.  the default
     is 5000.  Set ITL5=0 to omit this test.  (Note: not implemented in
     Ngspice).

`KEEPOPINFO'
     Retain the operating point information when either an AC,
     Distortion, or Pole-Zero analysis is run.  This is particularly
     useful if the circuit is large and you do not want to run a
     (redundant) ".OP" analysis.

`METHOD=name'
     sets the numerical integration method used by NGSPICE.  Possible
     names are "Gear" or "trapezoidal" (or just "trap").  The default
     is trapezoidal.

`PIVREL=x'
     resets the relative ratio between the largest column entry and an
     acceptable pivot value. The default value is 1.0e-3.  In the
     numerical pivoting algorithm the allowed minimum pivot value is
     determined by EPSREL=AMAX1(PIVREL*MAXVAL, PIVTOL) where MAXVAL is
     the maximum element in the column where a pivot is sought (partial
     pivoting).

`PIVTOL=x'
     resets the absolute minimum value for a matrix entry to be
     accepted as a pivot.  The default value is 1.0e-13.

`RELTOL=x'
     resets the relative error tolerance of the program.  The default
     value is 0.001 (0.1%).

`TEMP=x'
     Resets the operating temperature of the circuit.  The default
     value is 27 deg C (300 deg K).  TEMP can be overridden by a
     temperature specification on any temperature dependent instance.

`TNOM=x'
     resets the nominal temperature at which device parameters are
     measured.  The default value is 27 deg C (300 deg K).  TNOM can be
     overridden by a specification on any temperature dependent device
     model.

`TRTOL=x'
     resets the transient error tolerance.  The default value is 7.0.
     This parameter is an estimate of the factor by which NGSPICE
     overestimates the actual truncation error.

`TRYTOCOMPACT'
     Applicable only to the LTRA model.  When specified, the simulator
     tries to condense LTRA transmission lines' past history of input
     voltages and currents.

`VNTOL=x'
     resets the absolute voltage error tolerance of the program.  The
     default value is 1 microvolt.


   In addition, the following options have the listed effect when
operating in spice2 emulation mode:

`ACCT'
     causes accounting and run time statistics to be printed

`LIST'
     causes the summary listing of the input data to be printed

`NOMOD'
     suppresses the printout of the model parameters

`NOPAGE'
     suppresses page ejects

`NODE'
     causes the printing of the node table.

`OPTS'
     causes the option values to be printed.



File: ngspice.info,  Node: Initial Conditions,  Next: Analyses,  Prev: Simulator Variables (.OPTIONS),  Up: Analyses and Output Control

9.2 Initial Conditions
======================

* Menu:

* Specify Initial Node Voltage Guesses::
* Set Initial Conditions::


File: ngspice.info,  Node: Specify Initial Node Voltage Guesses,  Next: Set Initial Conditions,  Prev: Initial Conditions,  Up: Initial Conditions

9.2.1 .NODESET:  Specify Initial Node Voltage Guesses
-----------------------------------------------------

General form:

       .NODESET V(NODNUM)=VAL V(NODNUM)=VAL ...

   Examples:

       .NODESET V(12)=4.5 V(4)=2.23

   The Nodeset line helps the program find the dc or initial transient
solution by making a preliminary pass with the specified nodes held to
the given voltages.  The restriction is then released and the iteration
continues to the true solution.  The .NODESET line may be necessary for
convergence on bistable or a-stable circuits.  In general, this line
should not be necessary.


File: ngspice.info,  Node: Set Initial Conditions,  Prev: Specify Initial Node Voltage Guesses,  Up: Initial Conditions

9.2.2 .IC:  Set Initial Conditions
----------------------------------

General form:

       .IC V(NODNUM)=VAL V(NODNUM)=VAL ...

   Examples:

       .IC V(11)=5 V(4)=-5 V(2)=2.2

   The IC line is for setting transient initial conditions.  It has two
different interpretations, depending on whether the UIC parameter is
specified on the .TRAN control line.  Also, one should not confuse this
line with the .NODESET line.  The .NODESET line is only to help dc
convergence, and does not affect final bias solution (except for
multi-stable circuits).  The two interpretations of this line are as
follows:

  1. When the UIC parameter is specified on the .TRAN line, then the
     node voltages specified on the .IC control line are used to
     compute the capacitor, diode, BJT, JFET, and MOSFET initial
     conditions.  This is equivalent to specifying the IC=... parameter
     on each device line, but is much more convenient.  The IC=...
     parameter can still be specified and takes precedence over the .IC
     values.  Since no dc bias (initial transient) solution is computed
     before the transient analysis, one should take care to specify all
     dc source voltages on the .IC control line if they are to be used
     to compute device initial conditions.

  2. When the UIC parameter is not specified on the .TRAN control line,
     the dc bias (initial transient) solution is computed before the
     transient analysis.  In this case, the node voltages specified on
     the .IC control line is forced to the desired initial values
     during the bias solution.  During transient analysis, the
     constraint on these node voltages is removed.  This is the
     preferred method since it allows NGSPICE to compute a consistent
     dc solution.


File: ngspice.info,  Node: Analyses,  Next: Batch Output,  Prev: Initial Conditions,  Up: Analyses and Output Control

9.3 Analyses
============

* Menu:

* AC Small-Signal AC Analysis::
* DC Transfer Function::
* DISTRO Distortion Analysis::
* NOISE Noise Analysis::
* OP Operating Point Analysis::
* PZ Pole-Zero Analysis::
* SENS; DC or Small-Signal AC Sensitivity Analysis::
* TF Transfer Function Analysis::
* TRAN Transient Analysis::


File: ngspice.info,  Node: AC Small-Signal AC Analysis,  Next: DC Transfer Function,  Prev: Analyses,  Up: Analyses

9.3.1 .AC:  Small-Signal AC Analysis
------------------------------------

General form:

       .AC DEC ND FSTART FSTOP
       .AC OCT NO FSTART FSTOP
       .AC LIN NP FSTART FSTOP

   Examples:

       .AC DEC 10 1 10K
       .AC DEC 10 1K 100MEG
       .AC LIN 100 1 100HZ

   DEC stands for decade variation, and ND is the number of points per
decade.  OCT stands for octave variation, and NO is the number of points
per octave.  LIN stands for linear variation, and NP is the number of
points.  FSTART is the starting frequency, and FSTOP is the final
frequency.  If this line is included in the input file, NGSPICE performs
an AC analysis of the circuit over the specified frequency range.  Note
that in order for this analysis to be meaningful, at least one
independent source must have been specified with an ac value.


File: ngspice.info,  Node: DC Transfer Function,  Next: DISTRO Distortion Analysis,  Prev: AC Small-Signal AC Analysis,  Up: Analyses

9.3.2 .DC:  DC Transfer Function
--------------------------------

General form:

       .DC SRCNAM VSTART VSTOP VINCR [SRC2 START2 STOP2 INCR2]

   Examples:

       .DC VIN 0.25 5.0 0.25
       .DC VDS 0 10 .5 VGS 0 5 1
       .DC VCE 0 10 .25 IB 0 10U 1U
       .DC RLoad 1k 2k 100
       .DC TEMP -15 75 5

   The DC line defines the dc transfer curve source and sweep limits
(again with capacitors open and inductors shorted). SRCNAM is the name
of an independent voltage or current source, a resistor or the circuit
temperature.  VSTART, VSTOP, and VINCR are the starting, final, and
incrementing values respectively.  The first example causes the value
of the voltage source VIN to be swept from 0.25 Volts to 5.0 Volts in
increments of 0.25 Volts.  A second source (SRC2) may optionally be
specified with associated sweep parameters.  In this case, the first
source is swept over its range for each value of the second source.
This option can be useful for obtaining semiconductor device output
characteristics.  See the second example circuit description in
Appendix A.


File: ngspice.info,  Node: DISTRO Distortion Analysis,  Next: NOISE Noise Analysis,  Prev: DC Transfer Function,  Up: Analyses

9.3.3 .DISTO:  Distortion Analysis
----------------------------------

General form:

       .DISTO DEC ND FSTART FSTOP <F2OVERF1>
       .DISTO OCT NO FSTART FSTOP <F2OVERF1>
       .DISTO LIN NP FSTART FSTOP <F2OVERF1>

   Examples:

       .DISTO DEC 10 1kHz 100Mhz
       .DISTO DEC 10 1kHz 100Mhz 0.9

   The Disto line does a small-signal distortion analysis of the
circuit.  A multi-dimensional Volterra series analysis is done using
multi-dimensional Taylor series to represent the nonlinearities at the
operating point.  Terms of up to third order are used in the series
expansions.

   If the optional parameter F2OVERF1 is not specified, .DISTO does a
harmonic analysis - i.e., it analyses distortion in the circuit using
only a single input frequency F_1, which is swept as specified by
arguments of the .DISTO command exactly as in the .AC command.  Inputs
at this frequency may be present at more than one input source, and
their magnitudes and phases are specified by the arguments of the
DISTOF1 keyword in the input file lines for the input sources (see the
description for independent sources).  (The arguments of the DISTOF2
keyword are not relevant in this case).

   The analysis produces information about the A.C.  values of all node
voltages and branch currents at the harmonic frequencies 2F_1 and 3F_1,
vs. the input frequency F_1 as it is swept.  (A value of 1 (as a
complex distortion output) signifies \cos(2J(2F_1)t) at 2F_1 and
\cos(2J(3F_1)t) at 3F_1, using the convention that 1 at the input
fundamental frequency is equivalent to \cos(2JF_1t).)  The distortion
component desired (2F_1 or 3F_1) can be selected using commands in
nutmeg, and then printed or plotted.  (Normally, one is interested
primarily in the magnitude of the harmonic components, so the magnitude
of the AC distortion value is looked at).  It should be noted that
these are the A.C.  values of the actual harmonic components, and are
not equal to HD2 and HD3.  To obtain HD2 and HD3, one must divide by
the corresponding A.C. values at F_1, obtained from an .AC line.  This
division can be done using nutmeg commands.

   If the optional F2OVERF1 parameter is specified, it should be a real
number between (and not equal to) 0.0 and 1.0; in this case, .DISTO does
a spectral analysis.  It considers the circuit with sinusoidal inputs at
two different frequencies F_1 and F_2.  F_1 is swept according to the
.DISTO control line options exactly as in the .AC control line.  F_2 is
kept fixed at a single frequency as F_1 sweeps - the value at which it
is kept fixed is equal to F2OVERF1 times FSTART.  Each independent
source in the circuit may potentially have two (superimposed)
sinusoidal inputs for distortion, at the frequencies F_1 and F_2.  The
magnitude and phase of the F_1 component are specified by the arguments
of the DISTOF1 keyword in the source's input line (see the description
of independent sources); the magnitude and phase of the F_2 component
are specified by the arguments of the DISTOF2 keyword.  The analysis
produces plots of all node voltages/branch currents at the
intermodulation product frequencies F_1 + F_2, F_1 - F_2, and (2 F_1) -
F_2, vs the swept frequency F_1.  The IM product of interest may be
selected using the setplot command, and displayed with the print and
plot commands.  It is to be noted as in the harmonic analysis case, the
results are the actual AC voltages and currents at the intermodulation
frequencies, and need to be normalized with respect to .AC values to
obtain the IM parameters.

   If the DISTOF1 or DISTOF2 keywords are missing from the description
of an independent source, then that source is assumed to have no input
at the corresponding frequency.  The default values of the magnitude and
phase are 1.0 and 0.0 respectively.  The phase should be specified in
degrees.

   It should be carefully noted that the number F2OVERF1 should ideally
be an irrational number, and that since this is not possible in
practice, efforts should be made to keep the denominator in its
fractional representation as large as possible, certainly above 3, for
accurate results (i.e., if F2OVERF1 is represented as a fraction A/B,
where A and B are integers with no common factors, B should be as large
as possible; note that A < B because F2OVERF1 is constrained to be <
1).  To illustrate why, consider the cases where F2OVERF1 is 49/100 and
1/2.  In a spectral analysis, the outputs produced are at F_1 + F_2,
F_1 - F_2 and 2 F_1 - F_2.  In the latter case, F_1 - F_2 = F_2, so the
result at the F_1 - F_2 component is erroneous because there is the
strong fundamental F_2 component at the same frequency.  Also, F_1 +
F_2 = 2 F_1 - F_2 in the latter case, and each result is erroneous
individually.  This problem is not there in the case where F2OVERF1 =
49/100, because F_1-F_2 = 51/100 F_1 < > 49/100 F_1 = F_2.  In this
case, there are two very closely spaced frequency components at F_2 and
F_1 - F_2.  One of the advantages of the Volterra series technique is
that it computes distortions at mix frequencies expressed symbolically
(i.e. n F_1 + m F_2), therefore one is able to obtain the strengths of
distortion components accurately even if the separation between them is
very small, as opposed to transient analysis for example.  The
disadvantage is of course that if two of the mix frequencies coincide,
the results are not merged together and presented (though this could
presumably be done as a postprocessing step).  Currently, the
interested user should keep track of the mix frequencies himself or
herself and add the distortions at coinciding mix frequencies together
should it be necessary.


File: ngspice.info,  Node: NOISE Noise Analysis,  Next: OP Operating Point Analysis,  Prev: DISTRO Distortion Analysis,  Up: Analyses

9.3.4 .NOISE:  Noise Analysis
-----------------------------

General form:

          .NOISE V(OUTPUT <,REF>) SRC ( DEC | LIN | OCT ) PTS FSTART FSTOP
          + <PTS_PER_SUMMARY>

   Examples:

          .NOISE V(5) VIN DEC 10 1kHZ 100Mhz
          .NOISE V(5,3) V1 OCT 8 1.0 1.0e6 1

   The Noise line does a noise analysis of the circuit.  OUTPUT is the
node at which the total output noise is desired; if REF is specified,
then the noise voltage V(OUTPUT) - V(REF) is calculated.  By default,
REF is assumed to be ground.  SRC is the name of an independent source
to which input noise is referred.  PTS, FSTART and FSTOP are .AC type
parameters that specify the frequency range over which plots are
desired.  PTS_PER_SUMMARY is an optional integer; if specified, the
noise contributions of each noise generator is produced every
PTS_PER_SUMMARY frequency points.

   The .NOISE control line produces two plots - one for the Noise
Spectral Density curves and one for the total Integrated Noise over the
specified frequency range.  All noise voltages/currents are in squared
units (V^2 /Hz and A^2/Hz for spectral density, V^2 and A^2 for
integrated noise).


File: ngspice.info,  Node: OP Operating Point Analysis,  Next: PZ Pole-Zero Analysis,  Prev: NOISE Noise Analysis,  Up: Analyses

9.3.5 .OP:  Operating Point Analysis
------------------------------------

General form:

          .OP

   The inclusion of this line in an input file directs NGSPICE to
determine the dc operating point of the circuit with inductors shorted
and capacitors opened.  Note: a DC analysis is automatically performed
prior to a transient analysis to determine the transient initial
conditions, and prior to an AC small-signal, Noise, and Pole-Zero
analysis to determine the linearized, small-signal models for nonlinear
devices (see the KEEPOPINFO variable above).


File: ngspice.info,  Node: PZ Pole-Zero Analysis,  Next: SENS; DC or Small-Signal AC Sensitivity Analysis,  Prev: OP Operating Point Analysis,  Up: Analyses

9.3.6 .PZ:  Pole-Zero Analysis
------------------------------

General form:

          .PZ NODE1 NODE2 NODE3 NODE4 CUR POL
          .PZ NODE1 NODE2 NODE3 NODE4 CUR ZER
          .PZ NODE1 NODE2 NODE3 NODE4 CUR PZ
          .PZ NODE1 NODE2 NODE3 NODE4 VOL POL
          .PZ NODE1 NODE2 NODE3 NODE4 VOL ZER
          .PZ NODE1 NODE2 NODE3 NODE4 VOL PZ

   Examples:

          .PZ 1 0 3 0 CUR POL
          .PZ 2 3 5 0 VOL ZER
          .PZ 4 1 4 1 CUR PZ

   CUR stands for a transfer function of the type (output
voltage)/(input current) while VOL stands for a transfer function of
the type (output voltage)/(input voltage).  POL stands for pole
analysis only, ZER for zero analysis only and PZ for both.  This
feature is provided mainly because if there is a nonconvergence in
finding poles or zeros, then, at least the other can be found.
Finally, NODE1 and NODE2 are the two input nodes and NODE3 and NODE4
are the two output nodes.  Thus, there is complete freedom regarding
the output and input ports and the type of transfer function.

   In interactive mode, the command syntax is the same except that the
first field is PZ instead of .PZ.  To print the results, one should use
the command 'print all'.


File: ngspice.info,  Node: SENS; DC or Small-Signal AC Sensitivity Analysis,  Next: TF Transfer Function Analysis,  Prev: PZ Pole-Zero Analysis,  Up: Analyses

9.3.7 .SENS:  DC or Small-Signal AC Sensitivity Analysis
--------------------------------------------------------

General form:

          .SENS OUTVAR
          .SENS OUTVAR AC DEC ND FSTART FSTOP
          .SENS OUTVAR AC OCT NO FSTART FSTOP
          .SENS OUTVAR AC LIN NP FSTART FSTOP

   Examples:

          .SENS V(1,OUT)
          .SENS V(OUT) AC DEC 10 100 100k
          .SENS I(VTEST)

   The sensitivity of OUTVAR to all non-zero device parameters is
calculated when the SENS analysis is specified.  OUTVAR is a circuit
variable (node voltage or voltage-source branch current).  The first
form calculates sensitivity of the DC operating-point value of OUTVAR.
The second form calculates sensitivity of the AC values of OUTVAR.  The
parameters listed for AC sensitivity are the same as in an AC analysis
(see ".AC" above).  The output values are in dimensions of change in
output per unit change of input (as opposed to percent change in output
or per percent change of input).


File: ngspice.info,  Node: TF Transfer Function Analysis,  Next: TRAN Transient Analysis,  Prev: SENS; DC or Small-Signal AC Sensitivity Analysis,  Up: Analyses

9.3.8 .TF:  Transfer Function Analysis
--------------------------------------

General form:

          .TF OUTVAR INSRC

   Examples:

          .TF V(5, 3) VIN
          .TF I(VLOAD) VIN

   The TF line defines the small-signal output and input for the dc
small-signal analysis.  OUTVAR is the smallsignal output variable and
INSRC is the small-signal input source.  If this line is included,
NGSPICE computes the dc small-signal value of the transfer function
(output/input), input resistance, and output resistance.  For the first
example, NGSPICE would compute the ratio of V(5, 3) to VIN, the
small-signal input resistance at VIN, and the smallsignal output
resistance measured across nodes 5 and 3.


File: ngspice.info,  Node: TRAN Transient Analysis,  Prev: TF Transfer Function Analysis,  Up: Analyses

9.3.9 .TRAN:  Transient Analysis
--------------------------------

General form:

          .TRAN TSTEP TSTOP <TSTART <TMAX>>

   Examples:

          .TRAN 1NS 100NS
          .TRAN 1NS 1000NS 500NS
          .TRAN 10NS 1US

   TSTEP is the printing or plotting increment for lineprinter output.
For use with the post-processor, TSTEP is the suggested computing
increment.  TSTOP is the final time, and TSTART is the initial time.
If TSTART is omitted, it is assumed to be zero.  The transient analysis
always begins at time zero.  In the interval <zero, TSTART>, the
circuit is analyzed (to reach a steady state), but no outputs are
stored.  In the interval <TSTART, TSTOP>, the circuit is analyzed and
outputs are stored.  TMAX is the maximum stepsize that NGSPICE uses;
for default, the program chooses either TSTEP or (TSTOP-TSTART)/50.0,
whichever is smaller.  TMAX is useful when one wishes to guarantee a
computing interval which is smaller than the printer increment, TSTEP.

   UIC (use initial conditions) is an optional keyword which indicates
that the user does not want NGSPICE to solve for the quiescent
operating point before beginning the transient analysis.  If this
keyword is specified, NGSPICE uses the values specified using IC=... on
the various elements as the initial transient condition and proceeds
with the analysis.  If the .IC control line has been specified, then
the node voltages on the .IC line are used to compute the initial
conditions for the devices.  Look at the description on the .IC control
line for its interpretation when UIC is not specified.


File: ngspice.info,  Node: Batch Output,  Prev: Analyses,  Up: Analyses and Output Control

9.4 Batch Output
================

* Menu:

* SAVE::
* PRINT::
* PLOT::
* FOUR  Fourier Analysis of Transient Analysis  Output::


File: ngspice.info,  Node: SAVE,  Next: PRINT,  Prev: Batch Output,  Up: Batch Output

9.4.1 .SAVE Lines
-----------------

General form:

          .SAVE vector vector vector ...

   Examples:

          .SAVE i(vin) input output
          .SAVE @m1[id]

   The vectors listed on the .SAVE line are recorded in the rawfile for
use later with ngspice or nutmeg (nutmeg is just the data-analysis half
of ngspice, without the ability to simulate).  The standard vector
names are accepted.  If no .SAVE line is given, then the default set of
vectors are saved (node voltages and voltage source branch currents).
If .SAVE lines are given, only those vectors specified are saved.  For
more discussion on internal device data, see Appendix B.  See also the
section on the interactive command interpreter for information on how to
use the rawfile.


File: ngspice.info,  Node: PRINT,  Next: PLOT,  Prev: SAVE,  Up: Batch Output

9.4.2 .PRINT Lines
------------------

General form:

          .PRINT PRTYPE OV1 <OV2 ... OV8>

   Examples:

          .PRINT TRAN V(4) I(VIN)
          .PRINT DC V(2) I(VSRC) V(23, 17)
          .PRINT AC VM(4, 2) VR(7) VP(8, 3)

   The Print line defines the contents of a tabular listing of one to
eight output variables.  PRTYPE is the type of the analysis (DC, AC,
TRAN, NOISE, or DISTO) for which the specified outputs are desired.
The form for voltage or current output variables is the same as given
in the previous section for the print command; Spice2 restricts the
output variable to the following forms (though this restriction is not
enforced by Ngspice):

`V(N1<,N2>)'
     specifies the voltage difference between nodes N1 and N2.  If N2
     (and the preceding comma) is omitted, ground (0) is assumed.  See
     the print command in the previous section for more details.  For
     compatibility with spice2, the following five additional values
     can be accessed for the ac analysis by replacing the "V" in
     V(N1,N2) with:

                        VR    -    real part
                        VI    -    imaginary part
                        VM    -    magnitude
                        VP    -    phase
                        VDB   -    20  log10(magnitude)

`I(VXXXXXXX)'
     specifies the current flowing in the independent voltage source
     named VXXXXXXX.  Positive current flows from the positive node,
     through the source, to the negative node.  For the ac analysis,
     the corresponding replacements for the letter I may be made in the
     same way as described for voltage outputs.


   Output variables for the noise and distortion analyses have a
different general form from that of the other analyses.

   There is no limit on the number of .PRINT lines for each type of
analysis.


File: ngspice.info,  Node: PLOT,  Next: FOUR Fourier Analysis of Transient Analysis Output,  Prev: PRINT,  Up: Batch Output

9.4.3 .PLOT Lines
-----------------

General form:

          .PLOT PLTYPE OV1 <(PLO1, PHI1)> <OV2 <(PLO2, PHI2)> ... OV8>

   Examples:

          .PLOT DC V(4) V(5) V(1)
          .PLOT TRAN V(17, 5) (2, 5) I(VIN) V(17) (1, 9)
          .PLOT AC VM(5) VM(31, 24) VDB(5) VP(5)
          .PLOT DISTO HD2 HD3(R) SIM2
          .PLOT TRAN V(5, 3) V(4) (0, 5) V(7) (0, 10)

   The Plot line defines the contents of one plot of from one to eight
output variables.  PLTYPE is the type of analysis (DC, AC, TRAN, NOISE,
or DISTO) for which the specified outputs are desired.  The syntax for
the OVI is identical to that for the .PRINT line and for the plot
command in the interactive mode.

   The overlap of two or more traces on any plot is indicated by the
letter X.

   When more than one output variable appears on the same plot, the
first variable specified is printed as well as plotted.  If a printout
of all variables is desired, then a companion .PRINT line should be
included.

   There is no limit on the number of .PLOT  lines  specified for each
type of analysis.


File: ngspice.info,  Node: FOUR Fourier Analysis of Transient Analysis Output,  Prev: PLOT,  Up: Batch Output

9.4.4 .FOUR:  Fourier Analysis of Transient Analysis  Output
------------------------------------------------------------

General form:

          .FOUR FREQ OV1 <OV2 OV3 ...>

   Examples:

          .FOUR 100K  V(5)

   The Four (or Fourier) line controls whether NGSPICE performs a
Fourier analysis as a part of the transient analysis.  FREQ is the
fundamental frequency, and OV1, desired.  The Fourier analysis is
performed over the interval <TSTOP-period, TSTOP>, where TSTOP is the
final time specified for the transient analysis, and period is one
period of the fundamental frequency.  The dc component and the first
nine harmonics are determined.  For maximum accuracy, TMAX (see the
.TRAN line) should be set to period/100.0 (or less for very high-Q
circuits).


File: ngspice.info,  Node: Interactive Interpreter,  Next: Bibliography,  Prev: Analyses and Output Control,  Up: Top

10 Interactive Interpreter
**************************

Ngspice consists of a simulator and a front-end for data analysis and
plotting.  The front-end may be run as a separate "stand-alone" program
under the name Nutmeg.

   Nutmeg will read in the "raw" data output file created by ngspice -r
or with the write command in an interactive Ngspice session.  Nutmeg or
interactive Ngspice can plot data from a simulation on a graphics
terminal or a workstation display.  Most of the commands available in
the interactive Ngspice front end are available in nutmeg; where this is
not the case, ngspice-only commands have been marked with an asterisk
("*").  Note that the raw output file is different from the data that
Spice2 writes to the standard output, which may also be produced by
ngspice with the "-b" command line option.

   Ngspice and Nutmeg use the X Window System for plotting if they find
the environment variable DISPLAY.  Otherwise, a graphics-terminal
independent interface (MFB) is used.  If you are using X on a
workstation, the DISPLAY variable should already be set; if you want to
display graphics on a system different from the one you are running
Ngspice or Nutmeg on, DISPLAY should be of the form "machine:0.0".  See
the appropriate documentation on the X Window System for more details.

   Command Synopsis

     ngspice [ -n ] [ -t term ] [ -r rawfile] [ -b ] [ -i ] [ input file ... ]

     nutmeg [ - ] [ -n ] [ -t term ] [ datafile ... ]

   Options are:

`-'
     Don't try to load the default data file ("rawspice.raw") if no
     other files are given.  Nutmeg only.

`-n (or -N)'
     Don't try to source the file ".spiceinit" upon startup.  Normally
     ngspice and nutmeg try to find the file in the current directory,
     and if it is not found then in the user's home directory.

`-t term (or -T term)'
     The program is being run on a terminal with mfb name term.

`-b (or -B)'
     Run in batch mode.  Ngspice reads the default input source (e.g.
     keyboard) or reads the given input file and performs the analyses
     specified; output is either Spice2-like line-printer plots ("ascii
     plots") or a ngspice rawfile.  See the following section for
     details.  Note that if the input source is not a terminal (e.g.
     using the IO redirection notation of "<") Ngspice defaults to
     batch mode (-i overrides).  This option is valid for Ngspice only.

`-s (or -S)'
     Run in server mode.  This is like batch mode, except that a
     temporary rawfile is used and then written to the standard output,
     preceded by a line with a single "@", after the simulation is
     done.  This mode is used by the ngspice daemon.  This option is
     valid for Ngspice only.

`-i (or -I)'
     Run in interactive mode.  This is useful if the standard input is
     not a terminal but interactive mode is desired.  Command
     completion is not available unless the standard input is a
     terminal, however.  This option is valid for Ngspice only.

`-r rawfile (or -P rawfile)'
     Use rawfile as the default file into which the results of the
     simulation are saved.  This option is valid for Ngspice only.


   Further arguments to ngspice are taken to be Ngspice input files,
which are read and saved (if running in batch mode then they are run
immediately).  Ngspice accepts most Spice2 input file, and output ascii
plots, fourier analyses, and node printouts as specified in .plot,
.four, and .print cards.  If an out parameter is given on a .width
card, the effect is the same as set width = ....  Since Ngspice ascii
plots do not use multiple ranges, however, if vectors together on a
.plot card have different ranges they are not provide as much
information as they would in Spice2.  The output of Ngspice is also
much less verbose than Spice2, in that the only data printed is that
requested by the above cards.

   For nutmeg, further arguments are taken to be data files in binary or
ascii format (see sconvert(1)) which are loaded into nutmeg.  If the
file is in binary format, it may be only partially completed (useful for
examining Spice2 output before the simulation is finished).  One file
may contain any number of data sets from different analyses.

* Menu:

* Expressions::
* Command Interpretation::
* Commands::
* Variables::
* Bugs::


File: ngspice.info,  Node: Expressions,  Next: Command Interpretation,  Prev: Interactive Interpreter,  Up: Interactive Interpreter

10.1 Expressions, Functions, and Constants
==========================================

Ngspice and Nutmeg data is in the form of vectors: time, voltage, etc.
Each vector has a type, and vectors can be operated on and combined
algebraically in ways consistent with their types.  Vectors are normally
created when a data file is read in (see the load command below), and
when the initial datafile is loaded.  They can also be created with the
let command.

   An expression is an algebraic formula involving vectors and scalars
(a scalar is a vector of length 1) and the following operations:

                  +   -    *    /    ^   %

   % is the modulo operator, and the comma operator has two meanings:
if it is present in the argument list of a user definable function, it
serves to separate the arguments.  Otherwise, the term `x , y' is
synonymous with `x + j(y)'.

   Also available are the logical operations & (and), | (or), !  (not),
and the relational operations <, >, >=, <=, =, and <> (not equal).  If
used in an algebraic expression they work like they would in C,
producing values of 0 or 1.  The relational operators have the
following synonyms:

                            gt    >
                            lt    <
                            ge    >=
                            le    <=
                            ne    <>
                            eq    =
                            and   &
                            or    |
                            not   !

   These are useful when < and > might be confused with IO redirection
(which is almost always).

   The following functions are available:

`mag(vector)'
     The magnitude of vector

`ph(vector)'
     The phase of vector

`j(vector)'
     i (sqrt(-1)) times vector

`real(vector)'
     The real component of vector

`imag(vector)'
     The imaginary part of vector

`db(vector)'
     20 log10(mag(vector))

`log(vector)'
     The logarithm (base 10) of vector

`ln(vector)'
     The natural logarithm (base e) of vector

`exp(vector)'
     e to the vector power

`abs(vector)'
     The absolute value of vector.

`sqrt(vector)'
     The square root of vector.

`sin(vector)'
     The sine of vector.

`cos(vector)'
     The cosine of vector.

`tan(vector)'
     The tangent of vector.

`atan(vector)'
     The inverse tangent of vector.

`norm(vector)'
     The vector normalized to 1 (i.e, the largest magnitude of any
     component is 1).

`rnd(vector)'
     A vector with each component a random integer between 0 and the
     absolute value of the vectors's corresponding component.

`mean(vector)'
     The result is a scalar (a length 1 vec tor) that is the mean of the
     elements of vector.

`vector(number)'
     The result is a vector of length number, with elements 0, 1, ...
     number - 1.  If number is a vector then just the first element is
     taken, and if it isn't an integer then the floor of the magnitude
     is used.

`length(vector)'
     The length of vector.

`interpolate(plot.vector)'
     The result of interpolating the named vector onto the scale of the
     current plot.  This function uses the variable polydegree to
     determine the degree of interpolation.

`deriv(vector)'
     Calculates the derivative of the given vector.  This uses numeric
     differentiation by interpolating a polynomial and may not produce
     satisfactory results (particularly with iterated differentiation).
     The implementation only calculates the derivative with respect to
     the real component of that vector's scale.


   A vector may be either the name of a vector already defined or a
floating-point number (a scalar).  A number may be written in any format
acceptable to NGSPICE, such as 14.6Meg or -1.231e-4.  Note that you can
either use scientific notation or one of the abbreviations like MEG or
G, but not both.  As with NGSPICE, a number may have trailing alphabetic
characters after it.

   The notation expr [num] denotes the num'th element of expr.  For
multi-dimensional vectors, a vector of one less dimension is returned.
Also for multi-dimensional vectors, the notation expr[m][n] will return
the nth element of the mth subvector.  To get a subrange of a vector,
use the form expr[lower, upper].

   To reference vectors in a plot that is not the current plot (see the
setplot command, below), the notation plotname.vecname can be used.

   Either a plotname or a vector name may be the wildcard all.  If the
plotname is all, matching vectors from all plots are specified, and if
the vector name is all, all vectors in the specified plots are
referenced.  Note that you may not use binary operations on expressions
involving wildcards - it is not obvious what all + all should denote,
for instance.  Thus some (contrived) examples of expressions are:

          cos(TIME) + db(v(3))
          sin(cos(log([1 2 3 4 5 6 7 8 9 10])))
          TIME * rnd(v(9)) - 15 * cos(vin#branch) ^ [7.9e5 8]
          not ((ac3.FREQ[32] & tran1.TIME[10]) gt 3)

   Vector names in ngspice may have a name such as @name[param], where
name is either the name of a device instance or model.  This denotes the
value of the param parameter of the device or model.  See Appendix B for
details of what parameters are available.  The value is a vector of
length 1.  This function is also available with the show command, and is
available with variables for convenience for command scripts.

   There are a number of pre-defined constants in nutmeg.  They are:

`pi'
     J (3.14159...)

`e'
     The base of natural logarithms (2.71828...)

`c'
     The speed of light (299,792,500 m/sec)

`i'
     The square root of -1

`kelvin'
     Absolute 0 in Centigrade (-273.15 ^oC)

`echarge'
     The charge on an electron (1.6021918e-19 C)

`boltz'
     Boltzman's constant (1.3806226e-23)

`planck'
     Planck's constant (h = 6.626200e-34)


   These are all in MKS units.  If you have another variable with a name
that conflicts with one of these then it takes precedence.

* Menu:

* Command Interpretation::
* Commands::
* Variables::
* Bugs::


File: ngspice.info,  Node: Command Interpretation,  Next: Commands,  Prev: Expressions,  Up: Interactive Interpreter

10.2 Command Interpretation
===========================

If a word is typed as a command, and there is no built-in command with
that name, the directories in the sourcepath list are searched in order
for the file.  If it is found, it is read in as a command file (as if it
were sourced).  Before it is read, however, the variables argc and argv
are set to the number of words following the filename on the command
line, and a list of those words respectively.  After the file is
finished, these variables are unset.  Note that if a command file calls
another, it must save its argv and argc since they are altered.  Also,
command files may not be re-entrant since there are no local variables.
(Of course, the procedures may explicitly manipulate a stack...) This
way one can write scripts analogous to shell scripts for nutmeg and
Ngspice.

   Note that for the script to work with Ngspice, it must begin with a
blank line (or whatever else, since it is thrown away) and then a line
with .control on it.  This is an unfortunate result of the source
command being used for both circuit input and command file execution.
Note also that this allows the user to merely type the name of a
circuit file as a command and it is automatically run.  The commands
are executed immediately, without running any analyses that may be
specified in the circuit (to execute the analyses before the script
executes, include a "run" command in the script).

   There are various command scripts installed in
/usr/local/lib/spice/scripts (or whatever the path is on your machine),
and the default sourcepath includes this directory, so you can use these
command files (almost) like builtin commands.


File: ngspice.info,  Node: Commands,  Next: Variables,  Prev: Command Interpretation,  Up: Interactive Interpreter

10.3 Commands
=============

* Menu:

* AC::
* Alias::
* Alter::
* Asciiplot::
* Aspice::
* Bug::
* Cd::
* Destroy::
* DC::
* Define::
* Delete::
* Diff::
* Display::
* Echo::
* Edit::
* Fourier::
* Hardcopy::
* Help::
* History::
* Iplot::
* Jobs::
* Let::
* Linearize::
* Listing::
* Load::
* Op::
* Plot::
* Print::
* Quit::
* Rehash::
* Reset::
* Reshape::
* Resume::
* Rspice::
* Run::
* Rusage::
* Save::
* Sens::
* Set::
* Setcirc::
* Setplot::
* Settype::
* Shell::
* Shift::
* Show::
* Showmod::
* Source::
* Status::
* Step::
* Stop::
* Tf::
* Trace::
* Tran::
* Transpose::
* Unalias::
* Undefine::
* Unset::
* Version::
* Where::
* Write::
* Xgraph::
* While - End::
* Repeat - End::
* Dowhile - End::
* Foreach - End::
* If - Then - Else::
* Label::
* Goto::
* Continue::
* Break::


File: ngspice.info,  Node: AC,  Next: Alias,  Prev: Commands,  Up: Commands

10.3.1 Ac*: Perform an AC, small-signal frequency  response analysis
--------------------------------------------------------------------

General Form:

          ac ( DEC | OCT | LIN ) N Fstart Fstop

   Do an ac analysis.  See the previous sections of this manual for more
details.


File: ngspice.info,  Node: Alias,  Next: Alter,  Prev: AC,  Up: Commands

10.3.2 Alias:  Create an alias for a command
--------------------------------------------

General Form:

          alias [word] [text ...]

   Causes word to be aliased to text.  History substitutions may be
used, as in C-shell aliases.


File: ngspice.info,  Node: Alter,  Next: Asciiplot,  Prev: Alias,  Up: Commands

10.3.3 Alter*:  Change a device or model parameter
--------------------------------------------------

General Form:

          alter device value
          alter device parameter value [ parameter value ]

   Alter changes the value for a device or a specified parameter of a
device or model.  The first form is used by simple devices which have
one principal value (resistors, capacitors, etc.)  where the second form
is for more complex devices (bjt's, etc.).  Model parameters can be
changed with the second form if the name contains a "#".

   For specifying vectors as values, start the vector with "[",
followed by the values in the vector, and end with "]".  Be sure to
place a space between each of the values and before and after the "["
and "]".


File: ngspice.info,  Node: Asciiplot,  Next: Aspice,  Prev: Alter,  Up: Commands

10.3.4 Asciiplot: Plot values using old-style character plots
-------------------------------------------------------------

General Form:

          asciiplot plotargs

   Produce a line printer plot of the vectors.  The plot is sent to the
standard output, so you can put it into a file with asciiplot args ... >
file.  The set options width, height, and nobreak determine the width
and height of the plot, and whether there are page breaks, respectively.
Note that you will have problems if you try to asciiplot something with
an X-scale that isn't monotonic (i.e, something like sin(TIME) ),
because asciiplot uses a simple-minded linear interpolation.


File: ngspice.info,  Node: Aspice,  Next: Bug,  Prev: Asciiplot,  Up: Commands

10.3.5 Aspice: Asynchronous ngspice run
---------------------------------------

General Form:

          aspice input-file [output-file]

   Start a NGSPICE run, and when it is finished load the resulting data.
The raw data is kept in a temporary file.  If output-file is specified
then the diagnostic output is directed into that file, otherwise it is
thrown away.


File: ngspice.info,  Node: Bug,  Next: Cd,  Prev: Aspice,  Up: Commands

10.3.6 Bug:  Mail a bug report
------------------------------

General Form:

          bug

   Send a bug report.  Please include a short summary of the problem,
the version number and name of the operating system that you are
running, the version of ngspice that you are running, and the relevant
ngspice input file.  (If you have defined BUGADDR, the mail is
delivered to there.)


File: ngspice.info,  Node: Cd,  Next: Destroy,  Prev: Bug,  Up: Commands

10.3.7 Cd: Change directory
---------------------------

General Form:

          cd [directory]

   Change the current working directory to directory, or to the user's
home directory if none is given.


File: ngspice.info,  Node: Destroy,  Next: DC,  Prev: Cd,  Up: Commands

10.3.8 Destroy: Delete a data set
---------------------------------

General Form:

          destroy [plotnames | all]

   Release the memory holding the data for the  specified runs.


File: ngspice.info,  Node: DC,  Next: Define,  Prev: Destroy,  Up: Commands

10.3.9 Dc*: Perform a DC-sweep analysis
---------------------------------------

General Form:

          dc Source-Name Vstart Vstop Vincr [ Source2 Vstart2 Vstop2 Vincr2 ]

   Do a dc transfer curve analysis.  See the previous sections of this
manual for more details.


File: ngspice.info,  Node: Define,  Next: Delete,  Prev: DC,  Up: Commands

10.3.10 Define:  Define a function
----------------------------------

General Form:

          define function(arg1, arg2, ...) expression

   Define the user-definable function with the name function and
arguments arg1, arg2, ... to be expression, which may involve the
arguments.  When the function is later used, the arguments it is given
are substituted for the formal arguments when it is parsed.  If
expression is not present, any definition for function is printed, and
if there are no arguments to define then all currently active
definitions are printed.  Note that you may have different functions
defined with the same name but different arities.

   Some useful definitions are:

          define max(x,y) (x > y) * x + (x <= y) * y
          define min(x,y) (x < y) * x + (x >= y) * y


File: ngspice.info,  Node: Delete,  Next: Diff,  Prev: Define,  Up: Commands

10.3.11 Delete*: Remove a trace or breakpoint
---------------------------------------------

General Form:

          delete [ debug-number ... ]

   Delete the specified breakpoints and traces.  The debug numbers are
those shown by the status command (unless you do status > file, in which
case the debug numbers are not printed).


File: ngspice.info,  Node: Diff,  Next: Display,  Prev: Delete,  Up: Commands

10.3.12 Diff:  Compare vectors
------------------------------

General Form:

          diff plot1 plot2 [vec ...]

   Compare all the vectors in the specified plots, or only the named
vectors if any are given.  There are different vectors in the two plots,
or any values in the vectors differ significantly the difference is
reported.  The variable diff_abstol, diff_reltol, and diff_vntol are
used to determine a significant difference.


File: ngspice.info,  Node: Display,  Next: Echo,  Prev: Diff,  Up: Commands

10.3.13 Display:  List known vectors and types
----------------------------------------------

General Form:

          display [varname ...]

   Prints a summary of currently defined vectors, or of the names
specified.  The vectors are sorted by name unless the variable nosort is
set.  The information given is the name of the vector, the length, the
type of the vector, and whether it is real or complex data.
Additionally, one vector is labelled [scale].  When a command such as
plot is given without a vs argument, this scale is used for the X-axis.
It is always the first vector in a rawfile, or the first vector defined
in a new plot.  If you undefine the scale (i.e, let TIME = []), one of
the remaining vectors becomes the new scale (which is undetermined).


File: ngspice.info,  Node: Echo,  Next: Edit,  Prev: Display,  Up: Commands

10.3.14 Echo:  Print text
-------------------------

General Form:

          echo [text...]

   Echos the given text to the screen.


File: ngspice.info,  Node: Edit,  Next: Fourier,  Prev: Echo,  Up: Commands

10.3.15 Edit*: Edit the current circuit
---------------------------------------

General Form:

          edit [ file ]

   Print the current Ngspice input file into a file, call up the editor
on that file and allow the user to modify it, and then read it back in,
replacing the original file.  If a filename is given, then edit that
file and load it, making the circuit the current one.


File: ngspice.info,  Node: Fourier,  Next: Hardcopy,  Prev: Edit,  Up: Commands

10.3.16 Fourier: Perform a fourier transform
--------------------------------------------

General Form:

          fourier fundamental_frequency [value ...]

   Does a fourier analysis of each of the given values, using the first
10 multiples of the fundamental frequency (or the first nfreqs, if that
variable is set - see below).  The output is like that of the .four
Ngspice line.  The values may be any valid expression.  The values are
interpolated onto a fixed-space grid with the number of points given by
the fourgridsize variable, or 200 if it is not set.  The interpolation
is of degree polydegree if that variable is set, or 1.  If polydegree is
0, then no interpolation is done.  This is likely to give erroneous
results if the time scale is not monotonic, though.


File: ngspice.info,  Node: Hardcopy,  Next: Help,  Prev: Fourier,  Up: Commands

10.3.17 Hardcopy:  Save a plot to a file for printing
-----------------------------------------------------

General Form:

          hardcopy file plotargs

   Just like plot, except creates a file called file containing the
plot.  The file is an image in plot(5) format, and can be printed by
either the plot(1) program or lpr with the -g flag.


File: ngspice.info,  Node: Help,  Next: History,  Prev: Hardcopy,  Up: Commands

10.3.18 Help:  Print summaries of Ngspice commands
--------------------------------------------------

General Form:

          help [all] [command ...]

   Prints help.  If the argument all is given, a short description of
everything you could possibly type is printed.  If commands are given,
descriptions of those commands are printed.  Otherwise help for only a
few major commands is printed.


File: ngspice.info,  Node: History,  Next: Iplot,  Prev: Help,  Up: Commands

10.3.19 History:  Review previous commands
------------------------------------------

General Form:

          history [number]

   Print out the history, or the last number commands typed at the
keyboard.  Note: in Ngspice version 3a7 and earlier, all commands
(including ones read from files) were saved.


File: ngspice.info,  Node: Iplot,  Next: Jobs,  Prev: History,  Up: Commands

10.3.20 Iplot*: Incremental plot
--------------------------------

General Form:

          iplot [ node ...]

   Incrementally plot the values of the nodes while Ngspice runs.  The
iplot command can be used with the where command to find trouble spots
in a transient simulation.


File: ngspice.info,  Node: Jobs,  Next: Let,  Prev: Iplot,  Up: Commands

10.3.21 Jobs:  List active asynchronous ngspice runs
----------------------------------------------------

General Form:

          jobs

   Report on the asynchronous NGSPICE jobs currently running.  Nutmeg
checks to see if the jobs are finished every time you execute a command.
If it is done then the data is loaded and becomes available.


File: ngspice.info,  Node: Let,  Next: Linearize,  Prev: Jobs,  Up: Commands

10.3.22 Let:  Assign a value to a vector
----------------------------------------

General Form:

          let name = expr

   Creates a new vector called name with the value specified by expr, an
expression as described above.  If expr is [] (a zero-length vector)
then the vector becomes undefined.  Individual elements of a vector may
be modified by appending a subscript to name (ex. name[0]).  If there
are no arguments, let is the same as display.


File: ngspice.info,  Node: Linearize,  Next: Listing,  Prev: Let,  Up: Commands

10.3.23 Linearize*:  Interpolate to a linear scale
--------------------------------------------------

General Form:

          linearize vec ...

   Create a new plot with all of the vectors in the current plot, or
only those mentioned if arguments are given.  The new vectors are
interpolated onto a linear time scale, which is determined by the values
of tstep, tstart, and tstop in the currently active transient analysis.
The currently loaded input file must include a transient analysis (a
tran command may be run interactively before the last reset,
alternately), and the current plot must be from this transient analysis.
This command is needed because Ngspice doesn't output the results from a
transient analysis in the same manner that Spice2 did.


File: ngspice.info,  Node: Listing,  Next: Load,  Prev: Linearize,  Up: Commands

10.3.24 Listing*: Print a listing of the current circuit
--------------------------------------------------------

General Form:

          listing [logical] [physical] [deck] [expand]

   If the logical argument is given, the listing is with all
continuation lines collapsed into one line, and if the physical
argument is given the lines are printed out as they were found in the
file.  The default is logical.  A deck listing is just like the
physical listing, except without the line numbers it recreates the
input file verbatim (except that it does not preserve case).  If the
word expand is present, the circuit is printed with all subcircuits
expanded.


File: ngspice.info,  Node: Load,  Next: Op,  Prev: Listing,  Up: Commands

10.3.25 Load:  Load rawfile data
--------------------------------

General Form:

          load [filename] ...

   Loads either binary or ascii format rawfile data from the files
named.  The default filename is rawspice.raw, or the argument to the -r
flag if there was one.


File: ngspice.info,  Node: Op,  Next: Plot,  Prev: Load,  Up: Commands

10.3.26 Op*: Perform an operating point analysis
------------------------------------------------

General Form:

          op

   Do an operating point analysis.  See the previous sections of this
manual for more details.


File: ngspice.info,  Node: Plot,  Next: Print,  Prev: Op,  Up: Commands

10.3.27 Plot: Plot values on the display
----------------------------------------

General Form:

          plot exprs [ylimit ylo yhi] [xlimit xlo xhi] [xindices xilo xihi]
         [xcompress comp] [xdelta xdel] [ydelta ydel] [xlog] [ylog] [loglog]
         [vs xname] [xlabel word] [ylabel word] [title word] [samep]
         [linear]

   Plot the given exprs on the screen (if you are on a graphics
terminal).  The xlimit and ylimit arguments determine the high and low
x- and y-limits of the axes, respectively.  The xindices arguments
determine what range of points are to be plotted - everything between
the xilo'th point and the xihi'th point is plotted.  The xcompress
argument specifies that only one out of every comp points should be
plotted.  If an xdelta or a ydelta parameter is present, it specifies
the spacing between grid lines on the X- and Y-axis.  These parameter
names may be abbreviated to xl, yl, xind, xcomp, xdel, and ydel
respectively.

   The xname argument is an expression to use as the scale on the
x-axis. If xlog or ylog are present then the X or Y scale, respectively,
is logarithmic (loglog is the same as specifying both).  The xlabel and
ylabel arguments cause the specified labels to be used for the X and Y
axes, respectively.

   If samep is given, the values of the other parameters (other than
xname) from the previous plot, hardcopy, or asciiplot command is used
unless re-defined on the command line.

   The title argument is used in the place of the plot name at the
bottom of the graph.

   The linear keyword is used to override a default logscale plot (as in
the output for an AC analysis).

   Finally, the keyword polar to generate a polar plot.  To produce a
smith plot, use the keyword smith.  Note that the data is transformed,
so for smith plots you will see the data transformed by the function
(x-1)/(x+1).  To produce a polar plot with a smith grid but without
performing the smith transform, use the keyword smithgrid.


File: ngspice.info,  Node: Print,  Next: Quit,  Prev: Plot,  Up: Commands

10.3.28 Print:  Print values
----------------------------

General Form:

          print [col] [line] expr ...

   Prints the vector described by the expression expr.  If the col
argument is present, print the vectors named side by side.  If line is
given, the vectors are printed horizontally.  col is the default,
unless all the vectors named have a length of one, in which case line
is the default.  The options width, length, and nobreak are effective
for this command (see asciiplot).  If the expression is all, all of the
vectors available are printed.  Thus print col all > file prints
everything in the file in SPICE2 format.  The scale vector (time,
frequency) is always in the first column unless the variable
noprintscale is true.


File: ngspice.info,  Node: Quit,  Next: Rehash,  Prev: Print,  Up: Commands

10.3.29 Quit:  Leave Ngspice or Nutmeg
--------------------------------------

General Form:

          quit

   Quit nutmeg or ngspice.


File: ngspice.info,  Node: Rehash,  Next: Reset,  Prev: Quit,  Up: Commands

10.3.30 Rehash: Reset internal hash tables
------------------------------------------

General Form:

          rehash

   Recalculate the internal hash tables used when looking up UNIX
commands, and make all UNIX commands in the user's PATH available for
command completion.  This is useless unless you have set unixcom first
(see above).


File: ngspice.info,  Node: Reset,  Next: Reshape,  Prev: Rehash,  Up: Commands

10.3.31 Reset*: Reset an analysis
---------------------------------

General Form:

          reset

   Throw out any intermediate data in the circuit (e.g, after a
breakpoint or after one or more analyses have been done already), and
re-parse the input file.  The circuit can then be re-run from it's
initial state, overriding the affect of any set or alter commands.  In
Spice-3e and earlier versions this was done automatically by the run
command.


File: ngspice.info,  Node: Reshape,  Next: Resume,  Prev: Reset,  Up: Commands

10.3.32 Reshape: Alter the dimensionality or dimensions  of
-----------------------------------------------------------

a vector

   General Form:

          reshape vector vector ...
          or
          reshape vector vector ...  [ dimension, dimension, ...  ]
          or
          reshape vector vector ... [ dimension ][ dimension ] ...

   This command changes the dimensions of a vector or a set of vectors.
The final dimension may be left off and it will be filled in
automatically.  If no dimensions are specified, then the dimensions of
the first vector are copied to the other vectors.  An error message of
the form 'dimensions of x were inconsistent' can be ignored.


File: ngspice.info,  Node: Resume,  Next: Rspice,  Prev: Reshape,  Up: Commands

10.3.33 Resume*: Continue a simulation after a stop
---------------------------------------------------

General Form:

          resume

   Resume a simulation after a stop or interruption (control-C).


File: ngspice.info,  Node: Rspice,  Next: Run,  Prev: Resume,  Up: Commands

10.3.34 Rspice:  Remote ngspice submission
------------------------------------------

General Form:

          rspice input file

   Runs a NGSPICE remotely taking the input file as a NGSPICE input
file, or the current circuit if no argument is given.  Nutmeg or
Ngspice waits for the job to complete, and passes output from the
remote job to the user's standard output.  When the job is finished the
data is loaded in as with aspice.  If the variable rhost is set, nutmeg
connects to this host instead of the default remote Ngspice server
machine.  This command uses the "rsh" command and thereby requires
authentication via a ".rhosts" file or other equivalent method.  Note
that "rsh" refers to the "remote shell" program, which may be "remsh"
on your system; to override the default name of "rsh", set the variable
remote_shell.  If the variable rprogram is set, then rspice uses this
as the pathname to the program to run on the remote system.

   Note: rspice will not acknowledge elements that have been changed via
the "alter" or "altermod" commands.


File: ngspice.info,  Node: Run,  Next: Rusage,  Prev: Rspice,  Up: Commands

10.3.35 Run*: Run analysis from the input file
----------------------------------------------

General Form:

          run [rawfile]

   Run the simulation as specified in the input file.  If there were
any of the control lines .ac, .op, .tran, or .dc, they are executed.
The output is put in rawfile if it was given, in addition to being
available interactively.  In Spice-3e and earlier versions, the input
file would be re-read and any affects of the set or alter commands
would be reversed.  This is no longer the affect.


File: ngspice.info,  Node: Rusage,  Next: Save,  Prev: Run,  Up: Commands

10.3.36 Rusage: Resource usage
------------------------------

General Form:

          rusage [resource ...]

   Print resource usage statistics.  If any resources are given, just
print the usage of that resource.  Most resources require that a
circuit be loaded.  Currently valid resources are:

   elapsed           The amount of  time  elapsed  since  the  last
rusage                    elapsed call.   faults            Number of
page faults and context switches (BSD only).   space             Data
space used.   time              CPU time used so far.

   temp              Operating temperature.   tnom
Temperature at which device parameters were measured.   equations
 Circuit Equations

   time              Total Analysis Time  totiter           Total
iterations  accept            Accepted timepoints  rejected
Rejected timepoints

   loadtime          Time spent loading the circuit matrix and RHS.
reordertime       Matrix reordering time  lutime            L-U
decomposition time  solvetime         Matrix solve time

   trantime          Transient analysis time  tranpoints
Transient timepoints  traniter          Transient iterations
trancuriters      Transient iterations for the last time point*
tranlutime        Transient L-U decomposition time  transolvetime
Transient matrix solve time

   everything        All of the above.

   * listed incorrectly as "Transient iterations per point".


File: ngspice.info,  Node: Save,  Next: Sens,  Prev: Rusage,  Up: Commands

10.3.37 Save*:  Save a set of outputs
-------------------------------------

General Form:

          save [all | allv | alli | output ...]
          .save [all | allv | alli | output ...]

   Save a set of outputs, discarding the rest.  If a node has been
mentioned in a save command, it appears in the working plot after a run
has completed, or in the rawfile if ngspice is run in batch mode.  If a
node is traced or plotted (see below) it is also saved.  For backward
compatibility, if there are no save commands given, all outputs are
saved.

   When the keyword "all" or the keyword "allv", appears in the save
command, all node voltages, voltage source currents and inductor
currents are saved in addition to any other values listed. If the
keyword "alli" appears in the save command, all devices currents are
saved.

   Note: the current implementation saves only the currents of devices
which       have internal nodes, i.e. MOSFETs with non zero RD and RS;
BJTs with       non-zero RC, RB and RE; DIODEs with non-zero RS; etc.
Resistor and       capacitor currents are not saved with this option.
These deficiencies       will be addressed in a later revision.


File: ngspice.info,  Node: Sens,  Next: Set,  Prev: Save,  Up: Commands

10.3.38 Sens*:  Run a sensitivity analysis
------------------------------------------

General Form:

          sens output_variable
          sens output_variable ac ( DEC | OCT | LIN ) N Fstart Fstop

   Perform a Sensitivity analysis.  output_variable is either a node
voltage (ex. "v(1)" or "v(A,out)") or a current through a voltage source
(ex. "i(vtest)").  The first form calculates DC sensitivities, the
second form calculates AC sensitivies.  The output values are in
dimensions of change in output per unit change of input (as opposed to
percent change in output or per percent change of input).


File: ngspice.info,  Node: Set,  Next: Setcirc,  Prev: Sens,  Up: Commands

10.3.39 Set:  Set the value of a variable
-----------------------------------------

General Form:

          set [word]
          set [word = value] ...

   Set the value of word to be value, if it is present.  You can set any
word to be any value, numeric or string.  If no value is given then the
value is the boolean 'true'.

   The value of word may be inserted into a command by writing $word.
If a variable is set to a list of values that are enclosed in
parentheses (which must be separated from their values by white space),
the value of the variable is the list.

   The variables used by nutmeg are listed in the  following section.


File: ngspice.info,  Node: Setcirc,  Next: Setplot,  Prev: Set,  Up: Commands

10.3.40 Setcirc*: Change the current circuit
--------------------------------------------

General Form:

          setcirc [circuit name]

   The current circuit is the one that is used for the simulation
commands below.  When a circuit is loaded with the source command (see
below) it becomes the current circuit.


File: ngspice.info,  Node: Setplot,  Next: Settype,  Prev: Setcirc,  Up: Commands

10.3.41 Setplot:  Switch the current set of vectors
---------------------------------------------------

General Form:

          setplot [plotname]

   Set the current plot to the plot with the given name, or if no name
is given, prompt the user with a menu. (Note that the plots are named as
they are loaded, with names like tran1 or op2.  These names are shown by
the setplot and display commands and are used by diff, below.)  If the
"New plot" item is selected, the current plot becomes one with no
vectors defined.

   Note that here the word "plot" refers to a group of vectors that are
the result of one NGSPICE run.  When more than one file is loaded in,
or more than one plot is present in one file, nutmeg keeps them
separate and only shows you the vectors in the current plot.


File: ngspice.info,  Node: Settype,  Next: Shell,  Prev: Setplot,  Up: Commands

10.3.42 Settype:  Set the type of a vector
------------------------------------------

General Form:

          settype type vector ...

   Change the type of the named vectors to type.  Type names can be
found in the manual page for sconvert.


File: ngspice.info,  Node: Shell,  Next: Shift,  Prev: Settype,  Up: Commands

10.3.43 Shell:  Call the command interpreter
--------------------------------------------

General Form:

          shell [ command ]

   Call the operating system's command interpreter; execute the
specified command or call for interactive use.


File: ngspice.info,  Node: Shift,  Next: Show,  Prev: Shell,  Up: Commands

10.3.44 Shift:  Alter a list variable
-------------------------------------

General Form:

          shift [varname] [number]

   If varname is the name of a list variable, it is shifted to the left
by number elements (i.e, the number leftmost elements are removed).  The
default varname is argv, and the default number is 1.


File: ngspice.info,  Node: Show,  Next: Showmod,  Prev: Shift,  Up: Commands

10.3.45 Show*: List device state
--------------------------------

General Form:

          show devices [ : parameters ] , ...

   The show command prints out tables summarizing the operating
condition of selected devices (much like the spice2 operation point
summary).  If device is missing, a default set of devices are listed,
if device is a single letter, devices of that type are listed; if
device is a subcircuit name (beginning and ending in ":") only devices
in that subcircuit are shown (end the name in a double-":" to get
devices within sub-subcircuits recursively).  The second and third
forms may be combined ("letter:subcircuit:") or "letter:subcircuit::")
to select a specific type of device from a subcircuit.  A device's full
name may be specified to list only that device.  Finally, devices may
be selected by model by using the form "#modelname" or
":subcircuit#modelname" or "letter:subcircuit#modelname".

   If no parameters are specified, the values for a standard set of
parameters are listed.  If the list of parameters contains a "+", the
default set of parameters is listed along with any other specified
parameters.

   For both devices and parameters, the word "all" has the obvious
meaning.  Note: there must be spaces separating the ":" that divides
the device list from the parameter list.


File: ngspice.info,  Node: Showmod,  Next: Source,  Prev: Show,  Up: Commands

10.3.46 Showmod*: List model parameter values
---------------------------------------------

General Form:

          showmod models [ : parameters ] , ...

   The showmod command operates like the show command (above) but prints
out model parameter values.  The applicable forms for models are a
single letter specifying the device type letter, "letter:subckt:",
"modelname", ":subckt:modelname", or "letter:subcircuit:modelname".


File: ngspice.info,  Node: Source,  Next: Status,  Prev: Showmod,  Up: Commands

10.3.47 Source:  Read a Ngspice input file
------------------------------------------

General Form:

          source file

   For Ngspice: Read the Ngspice input file file.  Nutmeg and Ngspice
commands may be included in the file, and must be enclosed between the
lines .control and .endc.  These commands are executed immediately
after the circuit is loaded, so a control line of ac ...  works the
same as the corresponding .ac card.  The first line in any input file
is considered a title line and not parsed but kept as the name of the
circuit.  The exception to this rule is the file .spiceinit.  Thus, a
Ngspice command script must begin with a blank line and then with a
acters *# is considered a control line.  This makes it possible to
imbed commands in Ngspice input files that are ignored by earlier
versions of Spice2

   For Nutmeg: Reads commands from the file filename.  Lines beginning
with the character * are considered comments and ignored.


File: ngspice.info,  Node: Status,  Next: Step,  Prev: Source,  Up: Commands

10.3.48 Status*: Display breakpoint information
-----------------------------------------------

General Form:

          status

   Display all of the traces and breakpoints currently in effect.


File: ngspice.info,  Node: Step,  Next: Stop,  Prev: Status,  Up: Commands

10.3.49 Step*:  Run a fixed number of timepoints
------------------------------------------------

General Form:

          step [number]

   Iterate number times, or once, and then stop.


File: ngspice.info,  Node: Stop,  Next: Tf,  Prev: Step,  Up: Commands

10.3.50 Stop*:  Set a breakpoint
--------------------------------

General Form:

          stop [ after n] [ when value cond value ] ...

   Set a breakpoint.  The argument after n means stop after n iteration
number n, and the argument when value cond value means stop when the
first value is in the given relation with the second value, the possible
relations being

          eq   or   =    equal to
          ne   or   <>   not equal to
          gt   or   >    greater than
          lt   or   <    less than
          ge   or   >=   greater than or equal to
          le   or   <=   less than or equal to

   IO redirection is disabled for the stop command, since the relational
operations conflict with it (it doesn't produce any output anyway).  The
values above may be node names in the running circuit, or real values.
If more than one condition is given, e.g.  stop after 4 when v(1) > 4
when v(2) < 2, the conjunction of the conditions is implied.

10.3.51 Sysinfo:  Print system information
------------------------------------------

General Form:

          sysinfo

   The command prints system information useful for sending bug report
to developers.  Information consists of:

   * Name of the operating system,

   * Name of the node,

   * Current release of the operating system,

   * Current version of this release,

   * Name of hardware type.

   The example below shows the use of this command.

     ngspice 1 -> sysinfo
     Linux janus.wayout.net 2.4.20 #1 SMP Tue Jun 10 18:58:26 CEST 2003 i686
     ngspice 2 ->

     Note: This command may not be available on your environment, if it
     is not available, please send analogous information when submitting
     bug reports.


File: ngspice.info,  Node: Tf,  Next: Trace,  Prev: Stop,  Up: Commands

10.3.52 Tf*: Run a Transfer Function analysis
---------------------------------------------

General Form:

          tf output_node input_source

   The tf command performs a transfer function analysis, returning the
transfer function (output/input), output resistance, and input
resistance between the given output node and the given input source.
The analysis assumes a small-signal DC (slowly varying) input.


File: ngspice.info,  Node: Trace,  Next: Tran,  Prev: Tf,  Up: Commands

10.3.53 Trace*: Trace nodes
---------------------------

General Form:

          trace [ node ...]

   For every step of an analysis, the value of the node is printed.
Several traces may be active at once.  Tracing is not applicable for all
analyses.  To remove a trace, use the delete command.


File: ngspice.info,  Node: Tran,  Next: Transpose,  Prev: Trace,  Up: Commands

10.3.54 Tran*: Perform a transient analysis
-------------------------------------------

General Form:

          tran Tstep Tstop [ Tstart [ Tmax ] ] [ UIC ]

   Perform a transient analysis.  See the previous sections of this
manual for more details.


File: ngspice.info,  Node: Transpose,  Next: Unalias,  Prev: Tran,  Up: Commands

10.3.55 Transpose: Swap the elements in a multi-dimensional data set
--------------------------------------------------------------------

General Form:

          transpose vector vector ...

   This command transposes a multidimensional vector.  No analysis in
Ngspice produces multidimensional vectors, although the DC transfer
curve may be run with two varying sources.  You must use the "reshape"
command to reform the one-dimensional vectors into two dimensional
vectors.  In addition, the default scale is incorrect for plotting.
You must plot versus the vector corresponding to the second source, but
you must also refer only to the first segment of this second source
vector.  For example (circuit to produce the transfer characteristic of
a MOS transistor):

          ngspice > dc vgg 0 5 1 vdd 0 5 1
          ngspice > plot i(vdd)
          ngspice > reshape all [6,6]
          ngspice > transpose i(vdd) v(drain)
          ngspice > plot i(vdd) vs v(drain)[0]


File: ngspice.info,  Node: Unalias,  Next: Undefine,  Prev: Transpose,  Up: Commands

10.3.56 Unalias:  Retract an alias
----------------------------------

General Form:

          unalias [word ...]

   Removes any aliases present for the words.


File: ngspice.info,  Node: Undefine,  Next: Unset,  Prev: Unalias,  Up: Commands

10.3.57 Undefine:  Retract a definition
---------------------------------------

General Form:

          undefine function

   Definitions for the named user-defined functions are deleted.


File: ngspice.info,  Node: Unset,  Next: Version,  Prev: Undefine,  Up: Commands

10.3.58 Unset:  Clear a variable
--------------------------------

General Form:

          unset [word ...]

   Clear the value of the specified variable(s) (word).


File: ngspice.info,  Node: Version,  Next: Where,  Prev: Unset,  Up: Commands

10.3.59 Version:  Print the version of ngspice
----------------------------------------------

General Form:

          version [-s | -f | <version id>]

   Print out the version of _nutmeg_ that is running, if invoked
without argument or with `-s' or `-f'. If the argument is a  `<version
id>' (any string different from  `-s' or `-f' is considered a
`<version id>' ), the command checks to make sure that the arguments
match the current version of NGSPICE.  (This is mainly used as a
`Command:' line in rawfiles.)

   _Options description_
   * No option: The output of the command is the message you can see
     when running NGSPICE                  from the command line, no
     more no less.

   * `-s'(hort):  A shorter version of the message you see when calling
     NGSPICE from the                        command line.

   * `-f'(ull):   You may want to use this option if you want to know
     what extensions                         are included into the
     simulator and what compilation switches are 			active. A list of
     compilation options and included extensions is
     appended to the normal (not short) message. May be useful when
     sending 	                bug reports.

   The following example shows what the command returns is some
situations:

     ngspice 10 -> version
     ******
     ** ngspice-15 : Circuit level simulation program
     ** The U. C. Berkeley CAD Group
     ** Copyright 1985-1994, Regents of the University of California.
     ** Please submit bug-reports to: ngspice-devel@lists.sourceforge.net
     ** Creation Date: Sun Aug 24 00:35:57 CEST 2003
     ******
     ngspice 11 -> version 14
     Note: rawfile is version 14 (current version is 15)
     ngspice 12 -> version 15
     ngspice 13 ->

   *Note_for developers:* The option listing returned when `version' is
called with the `-f' option is built at compile time using `#ifdef'
blocks. When new compile switch are added, if you want them to appear
on the list, you have to modify the code in `misccoms.c'.


File: ngspice.info,  Node: Where,  Next: Write,  Prev: Version,  Up: Commands

10.3.60 Where:  Identify troublesome node or device
---------------------------------------------------

General Form:

          where

   When performing a transient or operating point analysis, the name of
the last node or device to cause non-convergence is saved.  The where
command prints out this information so that you can examine the circuit
and either correct the problem or make a bug report.  You may do this
either in the middle of a run or after the simulator has given up on the
analysis.  For transient simulation, the iplot command can be used to
monitor the progress of the analysis.  When the analysis slows down
severly or hangs, interrupt the simulator (with control-C) and issue the
where command.  Note that only one node or device is printed; there may
be problems with more than one node.


File: ngspice.info,  Node: Write,  Next: Xgraph,  Prev: Where,  Up: Commands

10.3.61 Write: Write data to a file
-----------------------------------

General Form:

          write [file] [exprs]

   Writes out the expressions to file.

   First vectors are grouped together by plots, and written out as such
(i.e, if the expression list contained three vectors from one plot and
two from another, then two plots are written, one with three vectors and
one with two).  Additionally, if the scale for a vector isn't present,
it is automatically written out as well.

   The default format is ascii, but this can be changed with the set
filetype command.  The default filename is rawspice.raw, or the argument
to the -r flag on the command line, if there was one, and the default
expression list is all.


File: ngspice.info,  Node: Xgraph,  Next: While - End,  Prev: Write,  Up: Commands

10.3.62 Xgraph: use the xgraph(1) program for plotting.
-------------------------------------------------------

General Form:

          xgraph file [exprs] [plot options]

   The ngspice/nutmeg xgraph command plots data like the plot command
but via xgraph, a popular X11 plotting program.

   If file is either "temp" or "tmp" a temporary file is used to hold
the data while being plotted.  For available plot options, see the plot
command.  All options except for polar or smith plots are supported.

10.4 Control Structures
=======================


File: ngspice.info,  Node: While - End,  Next: Repeat - End,  Prev: Xgraph,  Up: Commands

10.4.1 While - End
------------------

General Form:

          while condition
            statement
            ...
          end

   While condition, an arbitrary algebraic expression, is true, execute
the statements.


File: ngspice.info,  Node: Repeat - End,  Next: Dowhile - End,  Prev: While - End,  Up: Commands

10.4.2 Repeat - End
-------------------

General Form:

          repeat [number]
            statement
            ...
          end

   Execute the statements number times, or forever if no argument is
given.


File: ngspice.info,  Node: Dowhile - End,  Next: Foreach - End,  Prev: Repeat - End,  Up: Commands

10.4.3 Dowhile - End
--------------------

General Form:

          dowhile condition
            statement
            ...
          end

   The same as while, except that the condition is tested after the
statements are executed.


File: ngspice.info,  Node: Foreach - End,  Next: If - Then - Else,  Prev: Dowhile - End,  Up: Commands

10.4.4 Foreach - End
--------------------

General Form:

          foreach var value ...
            statement
            ...
          end

   The statements are executed once for each of the values, each time
with the variable var set to the current one.  (var can be accessed by
the $var notation - see below).


File: ngspice.info,  Node: If - Then - Else,  Next: Label,  Prev: Foreach - End,  Up: Commands

10.4.5 If - Then - Else
-----------------------

General Form:

          if condition
            statement
            ...
          else
            statement
            ...
          end

   If the condition is non-zero then the first set of statements are
executed, otherwise the second set.  The else and the second set of
statements may be omitted.


File: ngspice.info,  Node: Label,  Next: Goto,  Prev: If - Then - Else,  Up: Commands

10.4.6 Label
------------

General Form:

          label word

   If a statement of the form goto word is encountered, control is
transferred to this point, otherwise this is a no-op.


File: ngspice.info,  Node: Goto,  Next: Continue,  Prev: Label,  Up: Commands

10.4.7 Goto
-----------

General Form:

          goto word

   If a statement of the form label word is present in the block or an
enclosing block, control is transferred there.  Note that if the label
is at the top level, it must be before the goto statement (i.e, a
forward goto may occur only within a block).


File: ngspice.info,  Node: Continue,  Next: Break,  Prev: Goto,  Up: Commands

10.4.8 Continue
---------------

General Form:

          continue

   If there is a while, dowhile, or foreach block enclosing this
statement, control passes to the test, or in the case of foreach, the
next value is taken.  Otherwise an error results.


File: ngspice.info,  Node: Break,  Prev: Continue,  Up: Commands

10.4.9 Break
------------

General Form:

          break

   If there is a while, dowhile, or foreach block enclosing this
statement, control passes out of the block.  Otherwise an error results.

   Of course, control structures may be nested.  When a block is entered
and the input is the terminal, the prompt becomes a number of >'s
corresponding to the number of blocks the user has entered.  The current
control structures may be examined with the debugging command cdump.


File: ngspice.info,  Node: Variables,  Next: Bugs,  Prev: Commands,  Up: Interactive Interpreter

10.5 Variables
==============

The operation of both Nutmeg and Ngspice may be affected by setting
variables with the "set" command.  In addition to the variables
mentioned below, the set command in Ngspice also affect the behaviour of
the simulator via the options previously described under the section on
".OPTIONS".

   The variables meaningful to nutmeg which may be altered by the set
command are:

`diff_abstol'
     The absolute tolerance used by the diff command.  appendwrite
     Append to the file when a write command is is sued, if one already
     exists.

`colorN'
     These variables determine the colors used, if X is being run on a
     color display.  N may be between 0 and 15.  Color 0 is the
     background, color 1 is the grid and text color, and colors 2
     through 15 are used in order for vectors plot ted.  The value of
     the color variables should be names of colors, which may be found
     in the file /usr/lib/rgb.txt.

`combplot'
     Plot vectors by drawing a vertical line from each point to the
     X-axis, as opposed to joining the points.  Note that this option
     is subsumed in the plottype option, below.

`cpdebug'
     Print cshpar debugging information (must be com plied with the
     -DCPDEBUG flag).  Unsupported in the current release.

`debug'
     If set then a lot of debugging information is printed (must be
     compiled with the -DFTEDEBUG flag).  Unsupported in the current
     release.

`device'
     The name (`/dev/tty??') of the graphics device.  If this variable
     isn't set then the user's terminal is used.  To do plotting on
     another monitor you probably have to set both the device and term
     variables.  (If device is set to the name of a file, nutmeg dumps
     the graphics control codes into this file - this is useful for
     saving plots.)

`echo'
     Print out each command before it is executed.

`filetype'
     This can be either ascii or binary, and determines what format
     are.  The default is ascii.

`fourgridsize'
     How many points to use for interpolating into when doing fourier
     analysis.

`gridsize'
     If this variable is set to an integer, this number is used as the
     number of equally spaced points to use for the Y axis when
     plotting.  Otherwise the current scale is used (which may not have
     equally spaced points).  If the current scale isn't strictly
     monotonic, then this option has no effect.

`hcopydev'
     If this is set, when the hardcopy command is run the resulting
     file is automatically printed on the printer named hcopydev with
     the command `lpr -Phcopydev -g file'.

`hcopyfont'
     This variable specifies the font name for hardcopy output plots.
     The value is device dependent.

`hcopyfontsize'
     This is a scaling factor for the font used in hardcopy plots.

`hcopydevtype'
     This variable specifies the type of the printer output to use in
     the hardcopy command.  If hcopydevtype is not set, plot (5) format
     is assumed.  The standard distribution currently recognizes
     postscript as an alternative output for mat.  When used in
     conjunction with hcopydev, hcopydevtype should specify a format
     supported by the printer.

`height'
     The length of the page for asciiplot and print col.

`history'
     The number of events to save in the his tory list.

`lprplot5'
     This is a printf(3s) style format string used to specify the
     command to use for sending plot(5)-style plots to a printer or
     plotter.  The first parameter sup plied is the printer name, the
     second parameter supplied is a file name containing the plot.
     Both parameters are strings.  It is trivial to cause Ngspice to
     abort by supplying a unreasonable format string.

`lprps'
     This is a printf(3s) style format string used to specify the
     command to use for sending PostScript plots to a printer or
     plotter.  The first parameter supplied is the printer name, the
     second parameter supplied is a file name containing the plot.
     Both parameters are strings.  It is trivial to cause Ngspice to
     abort by supplying a unreasonable format string.

`nfreqs'
     The number of frequencies to compute in the fourier command.
     (Defaults to 10.)

`nobreak'
     Don't have asciiplot and print col break between pages.

`noasciiplotvalue'
     Don't print the first vector plotted to the left when doing an
     asciiplot.

`noclobber'
     Don't overwrite existing files when do ing IO redirection.

`noglob'
     Don't expand the global characters `*', `?', `[', and `]'.  This
     is the default.

`nogrid'
     Don't plot a grid when graphing curves (but do label the axes).

`nomoremode'
     If nomoremode is not set, whenever a large amount of data is being
     printed to the screen (e.g, the print or asciiplot commands), the
     output is stopped every screenful and continues when a carriage
     return is typed.  If nomoremode is set then data scrolls off the
     screen without check.

`nonomatch'
     If noglob is unset and a global expression cannot be matched, use
     the global characters literally instead of complaining.

`nosort'
     Don't have display sort the variable names.

`noprintscale'
     Don't print the scale in the leftmost column when a print col
     command is given.

`numdgt'
     The number of digits to print when printing tables of data
     (fourier, print col).  The default precision is 6 digits.  On the
     VAX, approximately 16 decimal digits are avail able using double
     precision, so numdgt should not be more than 16.  If the number is
     negative, one fewer digit is printed to ensure constant widths in
     tables.

`plottype'
     This should be one of normal, comb, or point:chars.  normal, the
     default, causes points to be plotted as parts of connected lines.
     comb causes a comb plot to be done (see the description of the
     combplot variable above).  point causes each point to be plotted
     separately - the chars are a list of characters that are used for
     each vector plotted.  If they are omitted then a de fault set is
     used.

`polydegree'
     The degree of the polynomial that the plot command should fit to
     the data.  If polydegree is N, then nutmeg fits a degree N
     polynomial to every set of N points and draw 10 intermediate
     points in between each end point.  If the points aren't monotonic,
     then it tries rotating the curve and reducing the degree until a
     fit is achieved.

`polysteps'
     The number of points to interpolate between every pair of points
     available when doing curve fitting.  The default is 10.

`program'
     The name of the current program (argv[0]).

`prompt'
     The prompt, with the character `!' replaced by the current event
     number.

`rawfile'
     The default name for rawfiles created.

`diff_reltol'
     The relative tolerance used by the diff command.

`remote_shell'
     Overrides the name used for generating rspice runs (default is
     "rsh").

`rhost'
     The machine to use for remote NGSPICE runs, in stead of the
     default one (see the description of the rspice command, below).

`rprogram'
     The name of the remote program to use in the rspice command.

`slowplot'
     Stop between each graph plotted and wait for the user to type
     return before continuing.

`sourcepath'
     A list of the directories to search when a source command is
     given.  The default is the current directory and the standard
     ngspice library (/usr/local/lib/ngspice, or whatever LIBPATH is
     #defined to in the Ngspice source.

`spicepath'
     The program to use for the aspice command.  The default is
     /cad/bin/spice.

`term'
     The mfb name of the current terminal.

`units'
     If this is degrees, then all the trig functions will use degrees
     instead of radians.

`unixcom'
     If a command isn't defined, try to execute it as a UNIX command.
     Setting this option has the effect of giving a rehash command,
     below.  This is useful for people who want to use nutmeg as a
     login shell.

`verbose'
     Be verbose.  This is midway between echo and de bug / cpdebug.

`diff _vntol'
     The absolute voltage tolerance used by the diff command.

`width'
     The width of the page for asciiplot and print col.

`x11lineararcs'
     Some X11 implementations have poor arc drawing.  If you set this
     option, Ngspice will plot using an approximation to the curve
     using straight lines.

`xbrushheight'
     The height of the brush to use if X is being run.

`xbrushwidth'
     The width of the brush to use if X is being run.

`xfont'
     The name of the X font to use when plotting data and entering
     labels.  The plot may not look good if this is a variable-width
     font.


   There are several set variables that Ngspice uses but Nutmeg does
not. They are:

`editor'
     The editor to use for the edit command.

`modelcard'
     The name of the model card (normally

`noaskquit'
     Do not check to make sure that there are no circuits suspended and
     no plots un saved.  Normally Ngspice warns the user when he tries
     to quit if this is the case.

`nobjthack'
     Assume that BJTs have 4 nodes.

`noparse'
     Don't attempt to parse input files when they are read in (useful
     for debugging).  Of course, they cannot be run if they are not
     parsed.  nosubckt Don't expand subcircuits.

`renumber'
     Renumber input lines when an input file has .include's.  subend
     The card to end subcircuits (normally

`subinvoke'
     The prefix to invoke subcircuits (nor mally x).  substart The card
     to begin subcircuits (normally


10.6 MISCELLANEOUS
==================

If there are subcircuits in the input file, Ngspice expands instances of
them.  A subcircuit is delimited by the cards .subckt and .ends, or
whatever the value of the variables substart and subend is,
respectively.  An instance of a subcircuit is created by specifying a
device with type 'x' - the device line is written

          xname node1 node2 ... subcktname

   where the nodes are the node names that replace the formal
parameters on the .subckt line.  All nodes that are not formal
parameters are prepended with the name given to the instance and a ':',
as are the names of the devices in the subcircuit.  If there are
several nested subcircuits, node and device names look like
subckt1:subckt2:...:name.  If the variable subinvoke is set, then it is
used as the prefix that specifies instances of subcircuits, instead of
'x'.

   Nutmeg occasionally checks to see if it is getting close to running
out of space, and warns the user if this is the case. (This is more
likely to be useful with the NGSPICE front end.)

   C-shell type quoting with "" and ", and backquote substitution may be
used.  Within single quotes, no further substitution (like history
substitution) is done, and within double quotes, the words are kept
together but further substitution is done.  Any text between backquotes
is replaced by the result of executing the text as a command to the
shell.

   Tenex-style ('set filec' in the 4.3 C-shell) command, filename, and
keyword completion is possible: If EOF (control-D) is typed after the
first character on the line, a list of the commands or possible
arguments is printed (If it is alone on the line it exits nutmeg).  If
escape is typed, then nutmeg tries to complete what the user has already
typed.  To get a list of all commands, the user should type <space> ^D.

   The values of variables may be used in commands by writing $varname
where the value of the variable is to appear.  The special variables $$
and $< refer to the process ID of the program and a line of input which
is read from the terminal when the variable is evaluated, respectively.
If a variable has a name of the form $&word, then word is considered a
vector (see above), and its value is taken to be the value of the
variable.  If $foo is a valid variable, and is of type list, then the
expression $foo[low-high] represents a range of elements.  Either the
upper index or the lower may be left out, and the reverse of a list may
be obtained with $foo[len-0].  Also, the notation $?foo evaluates to 1
if the variable foo is defined, 0 otherwise, and $#foo evaluates to the
number of elements in foo if it is a list, 1 if it is a number or
string, and 0 if it is a boolean variable.

   History substitutions, similar to C-shell history substitutions, are
also available - see the C-shell manual page for all of the details.

   The characters ~, {, and } have the same effects as they do in the
C-Shell, i.e., home directory and alternative expansion.  It is possible
to use the wildcard characters *, ?, [, and ] also, but only if you
unset noglob first.  This makes them rather useless for typing algebraic
expressions, so you should set noglob again after you are done with
wildcard expansion.  Note that the pattern [^abc] matchs all characters
except a, b, and c.

   IO redirection is available - the symbols >, >>, >&, >>&, and < have
the same effects as in the C-shell.

   You may type multiple commands on one line, separated by semicolons.

   If you want to use a different mfbcap file than the default (usually
~cad/lib/mfbcap), you have to set the environment variable SPICE_MFBCAP
before you start nutmeg or ngspice.  The -m option and the mfbcap
variable no longer work.

   If X is being used, the cursor may be positioned at any point on the
screen when the window is up and characters typed at the keyboard are
added to the window at that point.  The window may then be sent to a
printer using the xpr(1) program.

   Nutmeg can be run under VAX/VMS, as well as several other operating
systems.  Some features like command completion, expansion of *, ?, and
[], backquote substitution, the shell command, and so forth do not work.

   On some systems you have to respond to the -moreprompt during plot
with a carriage return instead of any key as you can do on UNIX.


File: ngspice.info,  Node: Bugs,  Prev: Variables,  Up: Interactive Interpreter

10.7 Bugs
=========

The label entry facilities are primitive.  You must be careful to type
slowly when entering labels - nutmeg checks for input once every
second, and can get confused if characters arrive faster.

   If you redefine colors after creating a plot window with X, and then
cause the window to be redrawn, it does not redraw in the correct
colors.

   When defining aliases like

          alias pdb plot db( '!:1' - '!:2' )

   you must be careful to quote the argument list substitutions in this
manner.  If you quote the whole argument it might not work properly.

   In a user-defined function, the arguments cannot be part of a name
that uses the plot.vec syntax.  For example:

          define check(v(1)) cos(tran1.v(1))

   does not work.

   If you type plot all all, or otherwise use a wildcard reference for
one plot twice in a command, the effect is unpredictable.

   The asciiplot command doesn't deal with log scales or the delta
keywords.

   Often the names of terminals recognized by MFB are different from
those in /etc/termcap.  Thus you may have to reset your terminal type
with the command

          set term = termname

   where termname is the name in the mfbcap file.

   The hardcopy command is useless on VMS and other systems without the
plot command, unless the user has a program that understands plot(5)
format.

   Ngspice recognizes all the notations used in SPICE2 .plot cards, and
translates vp(1) into ph(v(1)), and so forth.  However, if there are
spaces in these names it won't work.  Hence v(1, 2) and (-.5, .5) aren't
recognized.

   BJTs can have either 3 or 4 nodes, which makes it difficult for the
subcircuit expansion routines to decide what to rename.  If the fourth
parameter has been declared as a model name, then it is assumed that
there are 3 nodes, otherwise it is considered a node.  To disable this,
you can set the variable "nobjthack" which forces BJTs to have 4 nodes
(for the purposes of subcircuit expansion, at least).

   The @name[param] notation might not work with trace, iplot, etc.
yet.

   The first line of a command file (except for the .spiceinit file)
should be a comment, otherwise NGSPICE may create an empty circuit.

   Files specified on the command line are read before .spiceinit is
read.


File: ngspice.info,  Node: Bibliography,  Next: Example Circuits,  Prev: Interactive Interpreter,  Up: Top

11 Bibliography
***************

[1] A. Vladimirescu and S.  Liu, The Simulation of MOS Integrated
Circuits Using SPICE2 ERL Memo No. ERL M80/7, Electronics Research
Laboratory University of California, Berkeley, October 1980

   [2] T. Sakurai and A. R. Newton, A Simple MOSFET Model for Circuit
Analysis and its application to CMOS gate delay analysis and
series-connected MOSFET Structure ERL Memo No. ERL M90/19, Electronics
Research Labora tory, University of California, Berkeley, March 1990

   [3] B. J. Sheu, D. L. Scharfetter, and P.  K.  Ko, SPICE2
Implementation of BSIM ERL Memo No. ERL M85/42, Electronics Research
Labora tory University of California, Berkeley, May 1985

   [4] J. R. Pierret, A MOS Parameter Extraction Program for the BSIM
Model ERL Memo Nos.  ERL M84/99 and M84/100, Electronics Research
Laboratory University of California, Berkeley, November 1984

   [5] Min-Chie Jeng, Design and Modeling of Deep Submicrometer MOSFETSs
ERL Memo Nos. ERL M90/90, Electronics Research Labora tory University of
California, Berkeley, October 1990

   [6] Soyeon Park, Analysis and SPICE implementation of High
Temperature Effects on MOSFET, Master's thesis, University of
California, Berkeley, December 1986.

   [7] Clement Szeto, Simulator of Temperature Effects in MOS FETs
(STEIM), Master's thesis, University of California, Berkeley, May 1988.

   [8] J.S. Roychowdhury and D.O.  Pederson, Efficient Tran sient
Simulation of Lossy Interconnect, Proc. of the 28th ACM/IEEE Design
Automation Confer ence, June 17-21 1991, San Francisco

   [9] A. E. Parker and D. J. Skellern, An Improved FET Model for
Computer Simulators, IEEE Trans CAD, vol. 9, no. 5, pp. 551-553, May
1990.

   [10] R. Saleh and A. Yang, Editors, Simulation and Modeling, IEEE
Circuits and Devices, vol. 8, no. 3, pp.  7-8 and 49, May 1992

   [11] H.Statz et al., GaAs FET Device and Circuit Simulation in SPICE,
IEEE Transactions on Electron Devices, V34, Number 2, February, 1987
pp160-169.

   [12] Weidong Liu et al., BSIM3v3.2.2 MOSFET Model Users' Manual,
http://www-device.eecs.berkeley.edu/~bsim3/ftpv322/Mod_doc/V322manu.tar.Z

   [13] Weidong Lui et al. BSIM3.v3.2.3 MOSFET Model Users' Manual,
http://www-device.eecs.berkeley.edu/~bsim3/ftpv323/Mod_doc/BSIM323_manu.tar


File: ngspice.info,  Node: Example Circuits,  Next: Model and Device Parameters,  Prev: Bibliography,  Up: Top

12 Example Circuits
*******************

* Menu:

* Differential Pair::
* MOSFET Characterization::
* RTL Inverter::
* Four-Bit Binary Adder::
* Transmission-Line Inverter::


File: ngspice.info,  Node: Differential Pair,  Next: MOSFET Characterization,  Prev: Example Circuits,  Up: Example Circuits

12.1 Differential Pair
======================

The following deck determines the dc operating point of a simple
differential pair. In addition, the ac small-signal response is computed
over the frequency range 1Hz to 100MEGHz.

     SIMPLE DIFFERENTIAL PAIR
     VCC  7  0    12
     VEE  8  0    -12
     VIN  1  0    AC 1
     RS1  1  2    1K
     RS2  6  0    1K
     Q1   3  2  4 MOD1
     Q2   5  6  4 MOD1
     RC1  7  3    10K
     RC2  7  5    10K
     RE   4  8    10K
     .MODEL MOD1 NPN BF=50 VAF=50 IS=1.E-12 RB=100 CJC=.5PF TF=.6NS
     .TF V(5) VIN
     .AC DEC 10 1 100MEG
     .END


File: ngspice.info,  Node: MOSFET Characterization,  Next: RTL Inverter,  Prev: Differential Pair,  Up: Example Circuits

12.2 MOSFET Characterization
============================

The following deck computes the output characteristics of a MOSFET
device over the range 0-10V for VDS and 0-5V for VGS.

     MOS OUTPUT CHARACTERISTICS
     .OPTIONS NODE NOPAGE
     VDS  3  0
     VGS  2  0
     M1   1  2  0  0 MOD1 L=4U W=6U AD=10P AS=10P
     * VIDS MEASURES ID, WE COULD HAVE USED VDS, BUT ID WOULD BE NEGATIVE
     VIDS 3  1
     .MODEL MOD1 NMOS VTO=-2 NSUB=1.0E15 UO=550
     .DC VDS 0 10 .5 VGS 0 5 1
     .END


File: ngspice.info,  Node: RTL Inverter,  Next: Four-Bit Binary Adder,  Prev: MOSFET Characterization,  Up: Example Circuits

12.3 RTL Inverter
=================

The following deck determines the dc transfer curve and the transient
pulse response of a simple RTL inverter.  The input is a pulse from 0 to
5 Volts with delay, rise, and fall times of 2ns and a pulse width of
30ns.  The transient interval is 0 to 100ns, with printing to be done
every nanosecond.

     SIMPLE RTL INVERTER
     VCC  4  0    5
     VIN  1  0    PULSE 0 5 2NS 2NS 2NS 30NS
     RB   1  2    10K
     Q1   3  2  0 Q1
     RC   3  4    1K
     .MODEL Q1 NPN BF 20 RB 100 TF .1NS CJC 2PF
     .DC VIN 0 5 0.1
     .TRAN 1NS 100NS
     .END


File: ngspice.info,  Node: Four-Bit Binary Adder,  Next: Transmission-Line Inverter,  Prev: RTL Inverter,  Up: Example Circuits

12.4 Four-Bit Binary Adder
==========================

The following deck simulates a four-bit binary adder, using several
subcircuits to describe various pieces of the overall circuit.

     ADDER - 4 BIT ALL-NAND-GATE BINARY ADDER

     *** SUBCIRCUIT DEFINITIONS
     .SUBCKT NAND 1 2 3 4
     *   NODES:  INPUT(2), OUTPUT, VCC
     Q1        9  5  1 QMOD
     D1CLAMP   0  1    DMOD
     Q2        9  5  2 QMOD
     D2CLAMP   0  2    DMOD
     RB        4  5    4K
     R1        4  6    1.6K
     Q3        6  9  8 QMOD
     R2        8  0    1K
     RC        4  7    130
     Q4        7  6 10 QMOD
     DVBEDROP 10  3    DMOD
     Q5        3  8  0 QMOD
     .ENDS NAND

     .SUBCKT ONEBIT 1 2 3 4 5 6
     *   NODES:  INPUT(2), CARRY-IN, OUTPUT, CARRY-OUT, VCC
     X1   1  2  7  6   NAND
     X2   1  7  8  6   NAND
     X3   2  7  9  6   NAND
     X4   8  9 10  6   NAND
     X5   3 10 11  6   NAND
     X6   3 11 12  6   NAND
     X7  10 11 13  6   NAND
     X8  12 13  4  6   NAND
     X9  11  7  5  6   NAND
     .ENDS ONEBIT

     .SUBCKT TWOBIT 1 2 3 4 5 6 7 8 9
     *   NODES:  INPUT - BIT0(2) / BIT1(2), OUTPUT - BIT0 / BIT1,
     *           CARRY-IN, CARRY-OUT, VCC
     X1   1  2  7  5 10  9   ONEBIT
     X2   3  4 10  6  8  9   ONEBIT
     .ENDS TWOBIT

     .SUBCKT FOURBIT 1 2 3 4 5 6 7 8 9 10 11 12 13 14 15
     *   NODES:  INPUT - BIT0(2) / BIT1(2) / BIT2(2) / BIT3(2),
     *           OUTPUT - BIT0 / BIT1 / BIT2 / BIT3, CARRY-IN, CARRY-OUT, VCC
     X1   1  2  3  4  9 10 13 16 15   TWOBIT
     X2   5  6  7  8 11 12 16 14 15   TWOBIT
     .ENDS FOURBIT

     *** DEFINE NOMINAL CIRCUIT
     .MODEL DMOD D
     .MODEL QMOD NPN(BF=75 RB=100 CJE=1PF CJC=3PF)
     VCC   99  0   DC 5V
     VIN1A  1  0   PULSE(0 3 0 10NS 10NS   10NS   50NS)
     VIN1B  2  0   PULSE(0 3 0 10NS 10NS   20NS  100NS)
     VIN2A  3  0   PULSE(0 3 0 10NS 10NS   40NS  200NS)
     VIN2B  4  0   PULSE(0 3 0 10NS 10NS   80NS  400NS)
     VIN3A  5  0   PULSE(0 3 0 10NS 10NS  160NS  800NS)
     VIN3B  6  0   PULSE(0 3 0 10NS 10NS  320NS 1600NS)
     VIN4A  7  0   PULSE(0 3 0 10NS 10NS  640NS 3200NS)
     VIN4B  8  0   PULSE(0 3 0 10NS 10NS 1280NS 6400NS)
     X1     1  2  3  4  5  6  7  8  9 10 11 12  0 13 99 FOURBIT
     RBIT0  9  0   1K
     RBIT1 10  0   1K
     RBIT2 11  0   1K
     RBIT3 12  0   1K
     RCOUT 13  0   1K

     *** (FOR THOSE WITH MONEY (AND MEMORY) TO BURN)
     .TRAN 1NS 6400NS
     .END


File: ngspice.info,  Node: Transmission-Line Inverter,  Prev: Four-Bit Binary Adder,  Up: Example Circuits

12.5 Transmission-Line Inverter
===============================

The following deck simulates a transmission-line inverter.  Two
transmission-line elements are required since two propagation modes are
excited.  In the case of a coaxial line, the first line (T1) models the
inner conductor with respect to the shield, and the second line (T2)
models the shield with respect to the outside world.

     TRANSMISSION-LINE INVERTER
     V1   1  0         PULSE(0 1 0 0.1N)
     R1   1  2         50
     X1   2  0  0  4   TLINE
     R2   4  0         50

     .SUBCKT TLINE 1 2 3 4
     T1   1  2  3  4   Z0=50 TD=1.5NS
     T2   2  0  4  0   Z0=100 TD=1NS
     .ENDS TLINE

     .TRAN 0.1NS 20NS
     .END


File: ngspice.info,  Node: Model and Device Parameters,  Prev: Example Circuits,  Up: Top

13 Model and Device Parameters
******************************

The following tables summarize the parameters available on each of the
devices and models in (note that for some systems with limited memory,
output parameters are not available).  There are several tables for each
type of device supported by .  Input parameters to instances and models
are parameters that can occur on an instance or model definition line in
the form "keyword=value" where "keyword" is the parameter name as given
in the tables.  Default input parameters (such as the resistance of a
resistor or the capacitance of a capacitor) obviously do not need the
keyword specified.

   Output parameters are those additional parameters which are available
for many types of instances for the output of operating point and
debugging information.  These parameters are specified as
"@device[keyword]" and are available for the most recent point computed
or, if specified in a ".save" statement, for an entire simulation as a
normal output vector.  Thus, to monitor the gate-to-source capacitance
of a MOSFET, a command

        save @m1[cgs]

   given before a transient simulation causes the specified capacitance
value to be saved at each timepoint, and a subsequent command such as

        plot @m1[cgs]

   produces the desired plot.  (Note that the show command does not use
this format).

   Some variables are listed as both input and output, and their output
simply returns the previously input value, or the default value after
the simulation has been run.  Some parameter are input only because the
output system can not handle variables of the given type yet, or the
need for them as output variables has not been apparent.  Many such
input variables are available as output variables in a different format,
such as the initial condition vectors that can be retrieved as
individual initial condition values.  Finally, internally derived values
are output only and are provided for debugging and operating point
output purposes.

   Please note that these tables do not provide the detailed information
available about the parameters provided in the section on each device
and model, but are provided as a quick reference guide.

* Menu:

* Uniform RC line::
* Arbitrary Source::
* Bipolar Junction Transistor::
* BSIM1 Berkeley Short Channel IGFET Model::
* BSIM2 Berkeley Short Channel IGFET Model::
* Fixed capacitor::
* Current controlled current source::
* Linear current controlled current source::
* Current controlled ideal switch::
* Junction Diode model::
* Inductor::
* Mutual inductors::
* Independent current source::
* Junction Field effect transistor::
* Lossy transmission line::
* GaAs MESFET model::
* Level 1 MOSfet model::
* Level 2 MOSfet model::
* Level 3 MOSfet model::
* Level 6 MOSfet model::
* Simple linear resistor::
* Ideal voltage controlled switch::
* Lossless transmission line::
* Voltage controlled current source::
* Voltage controlled voltage source::
* Independent voltage source::


File: ngspice.info,  Node: Uniform RC line,  Next: Arbitrary Source,  Prev: Model and Device Parameters,  Up: Model and Device Parameters

13.1 URC:  Uniform R.C. line
============================


      ------------------------------------------------------------
     |          URC - instance parameters (input-output)         |
     |-----------------------------------------------------------+
     | l                 Length of transmission line             |
     | n                 Number of lumps                         |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |          URC - instance parameters (output-only)          |
     |-----------------------------------------------------------+
     | pos_node          Positive node of URC                    |
     | neg_node          Negative node of URC                    |
     | gnd               Ground node of URC                      |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |            URC - model parameters (input-only)            |
     |-----------------------------------------------------------+
     | urc               Uniform R.C. line model                 |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |           URC - model parameters (input-output)           |
     |-----------------------------------------------------------+
     | k                 Propagation constant                    |
     | fmax              Maximum frequency of interest           |
     | rperl             Resistance per unit length              |
     | cperl             Capacitance per unit length             |
     | isperl            Saturation current per length           |
     | rsperl            Diode resistance per length             |
      ------------------------------------------------------------


File: ngspice.info,  Node: Arbitrary Source,  Next: Bipolar Junction Transistor,  Prev: Uniform RC line,  Up: Model and Device Parameters

13.2 ASRC:  Arbitrary Source
============================


      ------------------------------------------------------------
     |          ASRC - instance parameters (input-only)          |
     |-----------------------------------------------------------+
     | i                 Current source                          |
     | v                 Voltage source                          |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |          ASRC - instance parameters (output-only)         |
     |-----------------------------------------------------------+
     | i                 Current through source                  |
     | v                 Voltage across source                   |
     | pos_node          Positive Node                           |
     | neg_node          Negative Node                           |
      ------------------------------------------------------------


File: ngspice.info,  Node: Bipolar Junction Transistor,  Next: BSIM1 Berkeley Short Channel IGFET Model,  Prev: Arbitrary Source,  Up: Model and Device Parameters

13.3 BJT:  Bipolar Junction Transistor
======================================


      ------------------------------------------------------------
     |           BJT - instance parameters (input-only)          |
     |-----------------------------------------------------------+
     | ic                Initial condition vector                |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |          BJT - instance parameters (input-output)         |
     |-----------------------------------------------------------+
     | off               Device initially off                    |
     | icvbe             Initial B-E voltage                     |
     | icvce             Initial C-E voltage                     |
     | area              Area factor                             |
     | temp              instance temperature                    |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |          BJT - instance parameters (output-only)          |
     |-----------------------------------------------------------+
     | colnode           Number of collector node                |
     | basenode          Number of base node                     |
     | emitnode          Number of emitter node                  |
     | substnode         Number of substrate node                |
      ------------------------------------------------------------
     | colprimenode      Internal collector node                 |
     | baseprimenode     Internal base node                      |
     | emitprimenode     Internal emitter node                   |
     | ic                Current at collector node               |
     |-----------------------------------------------------------+
       ib                Current at base node
     | ie                Emitter current                         |
     | is                Substrate current                       |
     | vbe               B-E voltage                             |
      ------------------------------------------------------------
     | vbc               B-C voltage                             |
     | gm                Small signal transconductance           |
     | gpi               Small signal input conductance - pi     |
     | gmu               Small signal conductance - mu           |
     |-----------------------------------------------------------+
     | gx                Conductance from base to internal base  |
     | go                Small signal output conductance         |
     | geqcb             d(Ibe)/d(Vbc)                           |
     | gccs              Internal C-S cap. equiv. cond.          |
      ------------------------------------------------------------
     | geqbx             Internal C-B-base cap. equiv. cond.     |
     | cpi               Internal base to emitter capactance     |
     | cmu               Internal base to collector capactiance  |
     | cbx               Base to collector capacitance           |
     |-----------------------------------------------------------+
     | ccs               Collector to substrate capacitance      |
     | cqbe              Cap. due to charge storage in B-E jct.  |
     | cqbc              Cap. due to charge storage in B-C jct.  |
     | cqcs              Cap. due to charge storage in C-S jct.  |
     | cqbx              Cap. due to charge storage in B-X jct.  |
     |                         continued                |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |     BJT - instance output-only parameters - continued
     |-----------------------------------------------------------+
     | cexbc             Total Capacitance in B-X junction       |
     | qbe               Charge storage B-E junction             |
     | qbc               Charge storage B-C junction             |
     | qcs               Charge storage C-S junction             |
     | qbx               Charge storage B-X junction             |
     | p                 Power dissipation                       |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |           BJT - model parameters (input-output)           |
     |-----------------------------------------------------------+
     | npn               NPN type device                         |
     | pnp               PNP type device                         |
     | is                Saturation Current                      |
     | bf                Ideal forward beta                      |
      ------------------------------------------------------------
     | nf                Forward emission coefficient            |
     | vaf               Forward Early voltage                   |
     | va                (null)                                  |
     | ikf               Forward beta roll-off corner current    |
     |-----------------------------------------------------------+
     | ik                (null)                                  |
     | ise               B-E leakage saturation current          |
     | ne                B-E leakage emission coefficient        |
     | br                Ideal reverse beta                      |
      ------------------------------------------------------------
     | nr                Reverse emission coefficient            |
     | var               Reverse Early voltage                   |
     | vb                (null)                                  |
     | ikr               reverse beta roll-off corner current    |
     |-----------------------------------------------------------+
     | isc               B-C leakage saturation current          |
     | nc                B-C leakage emission coefficient        |
     | rb                Zero bias base resistance               |
     | irb               Current for base resistance=(rb+rbm)/2  |
      ------------------------------------------------------------
     | rbm               Minimum base resistance                 |
     | re                Emitter resistance                      |
     | rc                Collector resistance                    |
     | cje               Zero bias B-E depletion capacitance     |
     |-----------------------------------------------------------+
     | vje               B-E built in potential                  |
     | pe                (null)                                  |
     | mje               B-E junction grading coefficient        |
     | me                (null)                                  |
      ------------------------------------------------------------
     | tf                Ideal forward transit time              |
     | xtf               Coefficient for bias dependence of TF   |
     | vtf               Voltage giving VBC dependence of TF     |
     | itf               High current dependence of TF           |
     |-----------------------------------------------------------+
     | ptf               Excess phase                            |
     | cjc               Zero bias B-C depletion capacitance     |
     | vjc               B-C built in potential                  |
     |                         continued                |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |      BJT - model input-output parameters - continued
     |-----------------------------------------------------------+
     | pc                (null)                                  |
     | mjc               B-C junction grading coefficient        |
     | mc                (null)                                  |
     | xcjc              Fraction of B-C cap to internal base    |
      ------------------------------------------------------------
     | tr                Ideal reverse transit time              |
     | cjs               Zero bias C-S capacitance               |
     | ccs               Zero bias C-S capacitance               |
     | vjs               Substrate junction built in potential   |
     |-----------------------------------------------------------+
     | ps                (null)                                  |
     | mjs               Substrate junction grading coefficient  |
     | ms                (null)                                  |
     | xtb               Forward and reverse beta temp. exp.     |
      ------------------------------------------------------------
     | eg                Energy gap for IS temp. dependency      |
     | xti               Temp. exponent for IS                   |
     | fc                Forward bias junction fit parameter     |
     | tnom              Parameter measurement temperature       |
     | kf                Flicker Noise Coefficient               |
     | af                Flicker Noise Exponent                  |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |            BJT - model parameters (output-only)           |
     |-----------------------------------------------------------+
     | type              NPN or PNP                              |
     | invearlyvoltf     Inverse early voltage:forward           |
     | invearlyvoltr     Inverse early voltage:reverse           |
     | invrollofff       Inverse roll off - forward              |
      ------------------------------------------------------------
     | invrolloffr       Inverse roll off - reverse              |
     | collectorconduct  Collector conductance                   |
     | emitterconduct    Emitter conductance                     |
     | transtimevbcfact  Transit time VBC factor                 |
     | excessphasefactor Excess phase fact.                      |
      ------------------------------------------------------------


File: ngspice.info,  Node: BSIM1 Berkeley Short Channel IGFET Model,  Next: BSIM2 Berkeley Short Channel IGFET Model,  Prev: Bipolar Junction Transistor,  Up: Model and Device Parameters

13.4 BSIM1:  Berkeley Short Channel IGFET Model
===============================================


      ------------------------------------------------------------
     |          BSIM1 - instance parameters (input-only)         |
     |-----------------------------------------------------------+
     | ic                Vector of DS,GS,BS initial voltages     |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |         BSIM1 - instance parameters (input-output)        |
     |-----------------------------------------------------------+
     | l                 Length                                  |
     | w                 Width                                   |
     | ad                Drain area                              |
     | as                Source area                             |
      ------------------------------------------------------------
     | pd                Drain perimeter                         |
     | ps                Source perimeter                        |
     | nrd               Number of squares in drain              |
     | nrs               Number of squares in source             |
     |-----------------------------------------------------------+
     | off               Device is initially off                 |
     | vds               Initial D-S voltage                     |
     | vgs               Initial G-S voltage                     |
     | vbs               Initial B-S voltage                     |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |           BSIM1 - model parameters (input-only)           |
     |-----------------------------------------------------------+
     | nmos              Flag to indicate NMOS                   |
     | pmos              Flag to indicate PMOS                   |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |          BSIM1 - model parameters (input-output)          |
     |-----------------------------------------------------------+
     | vfb               Flat band voltage                       |
     |lvfb               Length dependence of vfb                |
     | wvfb              Width dependence of vfb                 |
     | phi               Strong inversion surface potential      |
      ------------------------------------------------------------
     | lphi              Length dependence of phi                |
     | wphi              Width dependence of phi                 |
     | k1                Bulk effect coefficient 1               |
     | lk1               Length dependence of k1                 |
     |-----------------------------------------------------------+
     | wk1               Width dependence of k1                  |
     | k2                Bulk effect coefficient 2               |
     | lk2               Length dependence of k2                 |
     | wk2               Width dependence of k2                  |
      ------------------------------------------------------------
     | eta               VDS dependence of threshold voltage     |
     | leta              Length dependence of eta                |
     | weta              Width dependence of eta                 |
     | x2e               VBS dependence of eta                   |
     | lx2e              Length dependence of x2e                |
     |                         continued                |
      ------------------------------------------------------------


      ---------------------------------------------------------------------
     |          BSIM1 - model input-output parameters - continued         |
     |--------------------------------------------------------------------+
     |wx2e           Width dependence of x2e                              |
     |x3e            VDS dependence of eta                                |
     |lx3e           Length dependence of x3e                             |
     |wx3e           Width dependence of x3e                              |
      ---------------------------------------------------------------------
     |dl             Channel length reduction in um                       |
     |dw             Channel width reduction in um                        |
     |muz            Zero field mobility at VDS=0 VGS=VTH                 |
     |x2mz           VBS dependence of muz                                |
     |--------------------------------------------------------------------+
     |lx2mz          Length dependence of x2mz                            |
     |wx2mz          Width dependence of x2mz                             |
      mus            Mobility at VDS=VDD VGS=VTH, channel length modulation
     |lmus           Length dependence of mus                             |
      ---------------------------------------------------------------------
     |wmus           Width dependence of mus                              |
     |x2ms           VBS dependence of mus                                |
     |lx2ms          Length dependence of x2ms                            |
     |wx2ms          Width dependence of x2ms                             |
     |--------------------------------------------------------------------+
     |x3ms           VDS dependence of mus                                |
     |lx3ms          Length dependence of x3ms                            |
     |wx3ms          Width dependence of x3ms                             |
     |u0             VGS dependence of mobility                           |
      ---------------------------------------------------------------------
     |lu0            Length dependence of u0                              |
     |wu0            Width dependence of u0                               |
     |x2u0           VBS dependence of u0                                 |
     |lx2u0          Length dependence of x2u0                            |
     |--------------------------------------------------------------------+
     |wx2u0          Width dependence of x2u0                             |
     |u1             VDS dependece of mobility, velocity saturation       |
     |lu1            Length dependence of u1                              |
     |wu1            Width dependence of u1                               |
      ---------------------------------------------------------------------
     |x2u1           VBS dependence of u1                                 |
     |lx2u1          Length dependence of x2u1                            |
     |wx2u1          Width dependence of x2u1                             |
     |x3u1           VDS dependence of u1                                 |
     |--------------------------------------------------------------------+
     |lx3u1          Length dependence of x3u1                            |
     |wx3u1          Width dependence of x3u1                             |
     |n0             Subthreshold slope                                   |
      ln0            Length dependence of n0
      ---------------------------------------------------------------------
     |wn0            Width dependence of n0                               |
     |nb             VBS dependence of subthreshold slope                 |
     |lnb            Length dependence of nb                              |
     |wnb            Width dependence of nb                               |
     |--------------------------------------------------------------------+
     |nd             VDS dependence of subthreshold slope                 |
     |lnd            Length dependence of nd                              |
     |wnd            Width dependence of nd                               |
     |                              continued                             |
      ---------------------------------------------------------------------


      ---------------------------------------------------------------------------
     |          BSIM1 - model input-output parameters - continued            |
     |-----------------------------------------------------------------------+
     |tox         Gate oxide thickness in um                                 |
     |temp        Temperature in degree Celsius                              |
     |vdd         Supply voltage to specify mus                              |
     |cgso        Gate source overlap capacitance per unit channel width(m)  |
      ------------------------------------------------------------------------
     |cgdo        Gate drain overlap capacitance per unit channel width(m)   |
     |cgbo        Gate bulk overlap capacitance per unit channel length(m)   |
     |xpart       Flag for channel charge partitioning                       |
     |rsh         Source drain diffusion sheet resistance in ohm per square  |
     |-----------------------------------------------------------------------+
     |js          Source drain junction saturation current per unit area     |
     |pb          Source drain junction built in potential                   |
     |mj          Source drain bottom junction capacitance grading coefficient
     |pbsw        Source drain side junction capacitance built in potential  |
      ------------------------------------------------------------------------
     |mjsw        Source drain side junction capacitance grading coefficient |
     |cj          Source drain bottom junction capacitance per unit area     |
     |cjsw        Source drain side junction capacitance per unit area       |
     |wdf         Default width of source drain diffusion in um              |
     |dell        Length reduction of source drain diffusion                 |
      ------------------------------------------------------------------------


File: ngspice.info,  Node: BSIM2 Berkeley Short Channel IGFET Model,  Next: Fixed capacitor,  Prev: BSIM1 Berkeley Short Channel IGFET Model,  Up: Model and Device Parameters

13.5 BSIM2:  Berkeley Short Channel IGFET Model
===============================================


      ------------------------------------------------------------
     |          BSIM2 - instance parameters (input-only)         |
     |-----------------------------------------------------------+
     | ic                Vector of DS,GS,BS initial voltages     |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |         BSIM2 - instance parameters (input-output)        |
     |-----------------------------------------------------------+
     | l                 Length                                  |
     | w                 Width                                   |
     | ad                Drain area                              |
     | as                Source area                             |
      ------------------------------------------------------------
     | pd                Drain perimeter                         |
     | ps                Source perimeter                        |
     | nrd               Number of squares in drain              |
     | nrs               Number of squares in source             |
     |-----------------------------------------------------------+
     | off               Device is initially off                 |
     | vds               Initial D-S voltage                     |
     | vgs               Initial G-S voltage                     |
     | vbs               Initial B-S voltage                     |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |           BSIM2 - model parameters (input-only)           |
     |-----------------------------------------------------------+
     | nmos              Flag to indicate NMOS                   |
     | pmos              Flag to indicate PMOS                   |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |          BSIM2 - model parameters (input-output)          |
     |-----------------------------------------------------------+
     |vfb             Flat band voltage                          |
     |lvfb            Length dependence of vfb                   |
     |wvfb            Width dependence of vfb                    |
     |phi             Strong inversion surface potential         |
      ------------------------------------------------------------
     |lphi            Length dependence of phi                   |
     |wphi            Width dependence of phi                    |
     |k1              Bulk effect coefficient 1                  |
     |lk1             Length dependence of k1                    |
     |-----------------------------------------------------------+
     |wk1             Width dependence of k1                     |
     |k2              Bulk effect coefficient 2                  |
     |lk2             Length dependence of k2                    |
     |wk2             Width dependence of k2                     |
      ------------------------------------------------------------
     |eta0            VDS dependence of threshold voltage at VDD=0
     |leta0           Length dependence of eta0                  |
     |weta0           Width dependence of eta0                   |
     |etab            VBS dependence of eta                      |
     |-----------------------------------------------------------+
     |letab           Length dependence of etab                  |
     |wetab           Width dependence of etab                   |
     |dl              Channel length reduction in um             |
     |dw              Channel width reduction in um              |
      ------------------------------------------------------------
     |mu0             Low-field mobility, at VDS=0 VGS=VTH       |
     |mu0b            VBS dependence of low-field mobility       |
     |lmu0b           Length dependence of mu0b                  |
     |wmu0b           Width dependence of mu0b                   |
     |-----------------------------------------------------------+
     |mus0            Mobility at VDS=VDD VGS=VTH                |
     |lmus0           Length dependence of mus0                  |
     |wmus0           Width dependence of mus                    |
     |musb            VBS dependence of mus                      |
      ------------------------------------------------------------
     |lmusb           Length dependence of musb                  |
     |wmusb           Width dependence of musb                   |
     |mu20            VDS dependence of mu in tanh term          |
     |lmu20           Length dependence of mu20                  |
     |-----------------------------------------------------------+
     |wmu20           Width dependence of mu20                   |
     |mu2b            VBS dependence of mu2                      |
     |lmu2b           Length dependence of mu2b                  |
     |wmu2b           Width dependence of mu2b                   |
      ------------------------------------------------------------
     |mu2g            VGS dependence of mu2                      |
     |                         continued                |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |     BSIM2 - model input-output parameters - continued
     |-----------------------------------------------------------+
     | lmu2g             Length dependence of mu2g               |
     | wmu2g             Width dependence of mu2g                |
     | mu30              VDS dependence of mu in linear term     |
     | lmu30             Length dependence of mu30               |
      ------------------------------------------------------------
     | wmu30             Width dependence of mu30                |
     | mu3b              VBS dependence of mu3                   |
     | lmu3b             Length dependence of mu3b               |
     | wmu3b             Width dependence of mu3b                |
     |-----------------------------------------------------------+
     | mu3g              VGS dependence of mu3                   |
     | lmu3g             Length dependence of mu3g               |
     | wmu3g             Width dependence of mu3g                |
     | mu40              VDS dependence of mu in linear term     |
      ------------------------------------------------------------
     | lmu40             Length dependence of mu40               |
     | wmu40             Width dependence of mu40                |
     | mu4b              VBS dependence of mu4                   |
     | lmu4b             Length dependence of mu4b               |
     |-----------------------------------------------------------+
     | wmu4b             Width dependence of mu4b                |
     | mu4g              VGS dependence of mu4                   |
     | lmu4g             Length dependence of mu4g               |
     | wmu4g             Width dependence of mu4g                |
      ------------------------------------------------------------
     | ua0               Linear VGS dependence of mobility       |
     | lua0              Length dependence of ua0                |
     | wua0              Width dependence of ua0                 |
     | uab               VBS dependence of ua                    |
     |-----------------------------------------------------------+
     | luab              Length dependence of uab                |
     | wuab              Width dependence of uab                 |
     | ub0               Quadratic VGS dependence of mobility    |
     | lub0              Length dependence of ub0                |
      ------------------------------------------------------------
     | wub0              Width dependence of ub0                 |
     | ubb               VBS dependence of ub                    |
     | lubb              Length dependence of ubb                |
     | wubb              Width dependence of ubb                 |
     |-----------------------------------------------------------+
     | u10               VDS dependence of mobility              |
     | lu10              Length dependence of u10                |
       wu10              Width dependence of u100                |
     | u1b               VBS dependence of u1                    |
      ------------------------------------------------------------
     | lu1b              Length dependence of u1b                |
     | wu1b              Width dependence of u1b                 |
     | u1d               VDS dependence of u1                    |
     | lu1d              Length dependence of u1d                |
     |-----------------------------------------------------------+
     | wu1d              Width dependence of u1d                 |
     | n0                Subthreshold slope at VDS=0 VBS=0       |
     | ln0               Length dependence of n0                 |
     |                         continued                         |
      ------------------------------------------------------------


      --------------------------------------------------------------
     |           BSIM2 - model input-output parameters - continued  |
     |--------------------------------------------------------------+
     |wn0            Width dependence of n0                         |
     |nb             VBS dependence of n                            |
     |lnb            Length dependence of nb                        |
     |wnb            Width dependence of nb                         |
      --------------------------------------------------------------+
     |nd             VDS dependence of n                            |
     |lnd            Length dependence of nd                        |
     |wnd            Width dependence of nd                         |
     |vof0           Threshold voltage offset AT VDS=0 VBS=0        |
     |--------------------------------------------------------------+
     |lvof0          Length dependence of vof0                      |
     |wvof0          Width dependence of vof0                       |
     |vofb           VBS dependence of vof                          |
     |lvofb          Length dependence of vofb                      |
      --------------------------------------------------------------+
     |wvofb          Width dependence of vofb                       |
     |vofd           VDS dependence of vof                          |
     |lvofd          Length dependence of vofd                      |
     |wvofd          Width dependence of vofd                       |
     |--------------------------------------------------------------+
     |ai0            Pre-factor of hot-electron effect.             |
     |lai0           Length dependence of ai0                       |
     |wai0           Width dependence of ai0                        |
     |aib            VBS dependence of ai                           |
      --------------------------------------------------------------+
     |laib           Length dependence of aib                       |
     |waib           Width dependence of aib                        |
     |bi0            Exponential factor of hot-electron effect.     |
     |lbi0           Length dependence of bi0                       |
     |--------------------------------------------------------------+
     |wbi0           Width dependence of bi0                        |
     |bib            VBS dependence of bi                           |
     |lbib           Length dependence of bib                       |
     |wbib           Width dependence of bib                        |
      --------------------------------------------------------------+
     |vghigh         Upper bound of the cubic spline function.      |
     |lvghigh        Length dependence of vghigh                    |
     |wvghigh        Width dependence of vghigh                     |
     |vglow          Lower bound of the cubic spline function.      |
     |--------------------------------------------------------------+
     |lvglow         Length dependence of vglow                     |
     |wvglow         Width dependence of vglow                      |
     |tox            Gate oxide thickness in um                     |
     |temp           Temperature in degree Celcius                  |
      --------------------------------------------------------------+
     |vdd            Maximum Vds                                    |
     |vgg            Maximum Vgs                                    |
     |vbb            Maximum Vbs                                    |
     |cgso           Gate source overlap capacitance per unit       |
     |               channel width(m)                               |
     |--------------------------------------------------------------+
     |cgdo           Gate drain overlap capacitance                 |
     |               per unit channel width(m)                      |
     |cgbo           Gate bulk overlap capacitance                  |
     |               per unit channel length(m)                     |
     |xpart          Flag for channel charge partitioning           |
     |                               continued                      |
      ---------------------------------------------------------------


      ---------------------------------------------------------------
     |             BSIM2 - model input-output parameters            |
     |--------------------------------------------------------------+
     |rsh            Source drain diffusion sheet resistance        |
     |               in ohm per square                              |
     |js             Source drain junction saturation current       |
     |               per unit area                                  |
     |pb             Source drain junction built in potential       |
     |mj             Source drain bottom junction capacitance       |
     |               grading coefficient                            |
      --------------------------------------------------------------+
     |pbsw           Source drain side junction capacitance         |
     |               built in potential                             |
     |mjsw           Source drain side junction capacitance         |
     |               grading coefficient                            |
     |cj             Source drain bottom junction capacitance       |
     |               per unit area                                  |
     |cjsw           Source drain side junction capacitance         |
     |               per unit area                                  |
     |wdf            Default width of source drain diffusion in um  |
     |dell           Length reduction of source drain diffusion     |
      ---------------------------------------------------------------


File: ngspice.info,  Node: Fixed capacitor,  Next: Current controlled current source,  Prev: BSIM2 Berkeley Short Channel IGFET Model,  Up: Model and Device Parameters

13.6 Capacitor:  Fixed capacitor
================================


      ------------------------------------------------------------
     |       Capacitor - instance parameters (input-output)      |
     |-----------------------------------------------------------+
     | capacitance       Device capacitance                      |
     | ic                Initial capacitor voltage               |
     | w                 Device width                            |
     | l                 Device length                           |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |       Capacitor - instance parameters (output-only)       |
     |-----------------------------------------------------------+
     | i                 Device current                          |
     | p                 Instantaneous device power              |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |         Capacitor - model parameters (input-only)         |
     |-----------------------------------------------------------+
     | c                 Capacitor model                         |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |        Capacitor - model parameters (input-output)        |
     |-----------------------------------------------------------+
     | cj                Bottom Capacitance per area             |
     | cjsw              Sidewall capacitance per meter          |
     | defw              Default width                           |
     | narrow            width correction factor                 |
      ------------------------------------------------------------


File: ngspice.info,  Node: Current controlled current source,  Next: Linear current controlled current source,  Prev: Fixed capacitor,  Up: Model and Device Parameters

13.7 CCCS:  Current controlled current source
=============================================


      ------------------------------------------------------------
     |         CCCS - instance parameters (input-output)         |
     |-----------------------------------------------------------+
     | gain              Gain of source                          |
     | control           Name of controlling source              |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |          CCCS - instance parameters (output-only)         |
     |-----------------------------------------------------------+
     | neg_node          Negative node of source                 |
     | pos_node          Positive node of source                 |
     | i                 CCCS output current                     |
     | v                 CCCS voltage at output                  |
     | p                 CCCS power                              |
      ------------------------------------------------------------


File: ngspice.info,  Node: Linear current controlled current source,  Next: Current controlled ideal switch,  Prev: Current controlled current source,  Up: Model and Device Parameters

13.8 CCVS:  Linear current controlled current source
====================================================


      ------------------------------------------------------------
     |         CCVS - instance parameters (input-output)         |
     |-----------------------------------------------------------+
     | gain              Transresistance (gain)                  |
     | control           Controlling voltage source              |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |          CCVS - instance parameters (output-only)         |
     |-----------------------------------------------------------+
     | pos_node          Positive node of source                 |
     | neg_node          Negative node of source                 |
     | i                 CCVS output current                     |
     | v                 CCVS output voltage                     |
     | p                 CCVS power                              |
      ------------------------------------------------------------


File: ngspice.info,  Node: Current controlled ideal switch,  Next: Junction Diode model,  Prev: Linear current controlled current source,  Up: Model and Device Parameters

13.9 CSwitch:  Current controlled ideal switch
==============================================


      ------------------------------------------------------------
     |         CSwitch - instance parameters (input-only)        |
     |-----------------------------------------------------------+
     | on                Initially closed                        |
     | off               Initially open                          |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |        CSwitch - instance parameters (input-output)       |
     |-----------------------------------------------------------+
     | control           Name of controlling source              |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |        CSwitch - instance parameters (output-only)        |
     |-----------------------------------------------------------+
     | pos_node          Positive node of switch                 |
     | neg_node          Negative node of switch                 |
     | i                 Switch current                          |
     | p                 Instantaneous power                     |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |         CSwitch - model parameters (input-output)         |
     |-----------------------------------------------------------+
     | csw               Current controlled switch model         |
     | it                Threshold current                       |
     | ih                Hysteresis current                      |
     | ron               Closed resistance                       |
     | roff              Open resistance                         |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |          CSwitch - model parameters (output-only)         |
     |-----------------------------------------------------------+
     | gon               Closed conductance                      |
     | goff              Open conductance                        |
      ------------------------------------------------------------


File: ngspice.info,  Node: Junction Diode model,  Next: Inductor,  Prev: Current controlled ideal switch,  Up: Model and Device Parameters

13.10 Diode:  Junction Diode model
==================================


      ------------------------------------------------------------
     |         Diode - instance parameters (input-output)        |
     |-----------------------------------------------------------+
     | off               Initially off                           |
     | temp              Instance temperature                    |
     | ic                Initial device voltage                  |
     | area              Area factor                             |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |         Diode - instance parameters (output-only)         |
     |-----------------------------------------------------------+
     | vd                Diode voltage                           |
     | id                Diode current                           |
     | c                 Diode current                           |
     | gd                Diode conductance                       |
      ------------------------------------------------------------
     | cd                Diode capacitance                       |
     | charge            Diode capacitor charge                  |
     | capcur            Diode capacitor current                 |
     | p                 Diode power                             |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |           Diode - model parameters (input-only)           |
     |-----------------------------------------------------------+
     | d                 Diode model                             |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |          Diode - model parameters (input-output)          |
     |-----------------------------------------------------------+
     | is                Saturation current                      |
     | tnom              Parameter measurement temperature       |
     | rs                Ohmic resistance                        |
     | n                 Emission Coefficient                    |
      ------------------------------------------------------------
     | tt                Transit Time                            |
     | cjo               Junction capacitance                    |
     | cj0               (null)                                  |
     | vj                Junction potential                      |
     |-----------------------------------------------------------+
     | m                 Grading coefficient                     |
     | eg                Activation energy                       |
     | xti               Saturation current temperature exp.     |
     | kf                flicker noise coefficient               |
      ------------------------------------------------------------
     | af                flicker noise exponent                  |
     | fc                Forward bias junction fit parameter     |
     | bv                Reverse breakdown voltage               |
     | ibv               Current at reverse breakdown voltage    |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |           Diode - model parameters (output-only)          |
     |-----------------------------------------------------------+
     | cond              Ohmic conductance                       |
      ------------------------------------------------------------


File: ngspice.info,  Node: Inductor,  Next: Mutual inductors,  Prev: Junction Diode model,  Up: Model and Device Parameters

13.11 Inductor:  Inductors
==========================


      ------------------------------------------------------------
     |       Inductor - instance parameters (input-output)       |
     |-----------------------------------------------------------+
     | inductance        Inductance of inductor                  |
     | ic                Initial current through inductor        |
      ------------------------------------------------------------


      -------------------------------------------------------------
     |        Inductor - instance parameters (output-only)        |
     |------------------------------------------------------------+
     |flux           Flux through inductor                        |
     |v              Terminal voltage of inductor                 |
     |volt                                                        |
     |i              Current through the inductor                 |
     |current                                                     |
      p              instantaneous power dissipated by the inductor
     |                                                            |
      -------------------------------------------------------------


File: ngspice.info,  Node: Mutual inductors,  Next: Independent current source,  Prev: Inductor,  Up: Model and Device Parameters

13.12 mutual:  Mutual inductors
===============================


      ------------------------------------------------------------
     |        mutual - instance parameters (input-output)        |
     |-----------------------------------------------------------+
     | k                 Mutual inductance                       |
     | coefficient       (null)                                  |
     | inductor1         First coupled inductor                  |
     | inductor2         Second coupled inductor                 |
      ------------------------------------------------------------


File: ngspice.info,  Node: Independent current source,  Next: Junction Field effect transistor,  Prev: Mutual inductors,  Up: Model and Device Parameters

13.13 Isource:  Independent current source
==========================================


      ------------------------------------------------------------
     |         Isource - instance parameters (input-only)        |
     |-----------------------------------------------------------+
     | pulse             Pulse description                       |
     | sine              Sinusoidal source description           |
     | sin               Sinusoidal source description           |
     | exp               Exponential source description          |
      ------------------------------------------------------------
     | pwl               Piecewise linear description            |
     | sffm              single freq. FM description             |
     | ac                AC magnitude,phase vector               |
     | c                 Current through current source          |
     | distof1           f1 input for distortion                 |
     | distof2           f2 input for distortion                 |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |        Isource - instance parameters (input-output)       |
     |-----------------------------------------------------------+
     | dc                DC value of source                      |
     | acmag             AC magnitude                            |
     | acphase           AC phase                                |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |        Isource - instance parameters (output-only)        |
     |-----------------------------------------------------------+
     | neg_node          Negative node of source                 |
     | pos_node          Positive node of source                 |
       acreal            AC real part
     | acimag            AC imaginary part                       |
      ------------------------------------------------------------
     | function          Function of the source                  |
     | order             Order of the source function            |
     | coeffs            Coefficients of the source              |
     | v                 Voltage across the supply               |
     | p                 Power supplied by the source            |
      ------------------------------------------------------------


File: ngspice.info,  Node: Junction Field effect transistor,  Next: Lossy transmission line,  Prev: Independent current source,  Up: Model and Device Parameters

13.14 JFET:  Junction Field effect transistor
=============================================


      ------------------------------------------------------------
     |         JFET - instance parameters (input-output)         |
     |-----------------------------------------------------------+
     | off               Device initially off                    |
     | ic                Initial VDS,VGS vector                  |
     | area              Area factor                             |
     | ic-vds            Initial D-S voltage                     |
     | ic-vgs            Initial G-S volrage                     |
     | temp              Instance temperature                    |
      ------------------------------------------------------------


      ---------------------------------------------------------------
     |           JFET - instance parameters (output-only)           |
     |--------------------------------------------------------------+
     |drain-node       Number of drain node                         |
     |gate-node        Number of gate node                          |
     |source-node      Number of source node                        |
     |drain-prime-node Internal drain node                          |
      ---------------------------------------------------------------
     |source-prime-nodeInternal source node                         |
     |vgs              Voltage G-S                                  |
     |vgd              Voltage G-D                                  |
     |ig               Current at gate node                         |
     |--------------------------------------------------------------+
     |id               Current at drain node                        |
     |is               Source current                               |
     |igd              Current G-D                                  |
     |gm               Transconductance                             |
      ---------------------------------------------------------------
     |gds              Conductance D-S                              |
     |ggs              Conductance G-S                              |
     |ggd              Conductance G-D                              |
     |qgs              Charge storage G-S junction                  |
     |--------------------------------------------------------------+
     |qgd              Charge storage G-D junction                  |
      cqgs             Capacitance due to charge storage G-S junction
     |                                                              |
      cqgd             Capacitance due to charge storage G-D junction
     |p                Power dissipated by the JFET                 |
      ---------------------------------------------------------------


      ------------------------------------------------------------
     |           JFET - model parameters (input-output)          |
     |-----------------------------------------------------------+
     | njf               N type JFET model                       |
     | pjf               P type JFET model                       |
     | vt0               Threshold voltage                       |
     | vto               (null)                                  |
      ------------------------------------------------------------
     | beta              Transconductance parameter              |
     | lambda            Channel length modulation param.        |
     | rd                Drain ohmic resistance                  |
     | rs                Source ohmic resistance                 |
     | cgs               G-S junction capacitance                |
     |                         continued                         |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |      JFET - model input-output parameters - continued
     |-----------------------------------------------------------+
     | cgd               G-D junction cap                        |
     | pb                Gate junction potential                 |
     | is                Gate junction saturation current        |
     | fc                Forward bias junction fit param.        |
      ------------------------------------------------------------
     | b                 Doping tail parameter                   |
     | tnom              parameter measurement temperature       |
     | kf                Flicker Noise Coefficient               |
     | af                Flicker Noise Exponent                  |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |           JFET - model parameters (output-only)           |
     |-----------------------------------------------------------+
     | type              N-type or P-type JFET model             |
     | gd                Drain conductance                       |
     | gs                Source conductance                      |
      ------------------------------------------------------------


File: ngspice.info,  Node: Lossy transmission line,  Next: GaAs MESFET model,  Prev: Junction Field effect transistor,  Up: Model and Device Parameters

13.15 LTRA:  Lossy transmission line
====================================


      ------------------------------------------------------------
     |          LTRA - instance parameters (input-only)          |
     |-----------------------------------------------------------+
     | ic                Initial condition vector:v1,i1,v2,i2    |
      ------------------------------------------------------------

      ------------------------------------------------------------
     |         LTRA - instance parameters (input-output)         |
     |-----------------------------------------------------------+
     | v1                Initial voltage at end 1                |
     | v2                Initial voltage at end 2                |
     | i1                Initial current at end 1                |
     | i2                Initial current at end 2                |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |          LTRA - instance parameters (output-only)         |
     |-----------------------------------------------------------+
     | pos_node1         Positive node of end 1 of t-line        |
     | neg_node1         Negative node of end 1 of t.line        |
     | pos_node2         Positive node of end 2 of t-line        |
     | neg_node2         Negative node of end 2 of t-line        |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |           LTRA - model parameters (input-output)          |
     |-----------------------------------------------------------+
     |ltra            LTRA model                                 |
     |r               Resistance per metre                       |
     |l               Inductance per metre                       |
     |g               (null)                                     |
      ------------------------------------------------------------
     |c               Capacitance per metre                      |
     |len             length of line                             |
     |nocontrol       No timestep control                        |
     |steplimit       always limit timestep to 0.8*(delay of line)
     |                         continued                         |
      ------------------------------------------------------------

      ---------------------------------------------------------------------
     |                 LTRA - model input-output parameters - continued    |
     |---------------------------------------------------------------------+
     |nosteplimit    don't always limit timestep to 0.8*(delay of line)    |
     |lininterp      use linear interpolation                              |
     |quadinterp     use quadratic interpolation                           |
     |mixedinterp    use linear interpolation if quadratic results         |
     |               look unacceptable                                     |
      ---------------------------------------------------------------------
     |truncnr        use N-R iterations for step calculation in LTRAtrunc  |
     |truncdontcut   don't limit timestep to keep impulse response         |
     |               calculation errors low                                |
     |compactrel     special reltol for straight line checking             |
     |compactabs     special abstol for straight line checking             |
      ---------------------------------------------------------------------


      ------------------------------------------------------------
     |           LTRA - model parameters (output-only)           |
     |-----------------------------------------------------------+
     | rel               Rel. rate of change of deriv. for bkpt  |
     | abs               Abs. rate of change of deriv. for bkpt  |
      ------------------------------------------------------------


File: ngspice.info,  Node: GaAs MESFET model,  Next: Level 1 MOSfet model,  Prev: Lossy transmission line,  Up: Model and Device Parameters

13.16 MES:  GaAs MESFET model
=============================


      ------------------------------------------------------------
     |          MES - instance parameters (input-output)         |
     |-----------------------------------------------------------+
     | area              Area factor                             |
     | icvds             Initial D-S voltage                     |
     | icvgs             Initial G-S voltage                     |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |          MES - instance parameters (output-only)          |
     |-----------------------------------------------------------+
     |off            Device initially off                        |
     |dnode          Number of drain node                        |
     |gnode          Number of gate node                         |
     |snode          Number of source node                       |
      ------------------------------------------------------------
     |dprimenode     Number of internal drain node               |
     |sprimenode     Number of internal source node              |
     |vgs            Gate-Source voltage                         |
     |vgd            Gate-Drain voltage                          |
     |-----------------------------------------------------------+
     |cg             Gate capacitance                            |
     |cd             Drain capacitance                           |
     |cgd            Gate-Drain capacitance                      |
     |gm             Transconductance                            |
      ------------------------------------------------------------
     |gds            Drain-Source conductance                    |
     |ggs            Gate-Source conductance                     |
     |ggd            Gate-Drain conductance                      |
     |cqgs           Capacitance due to gate-source charge storage
     |-----------------------------------------------------------+
     |cqgd           Capacitance due to gate-drain charge storage|
     |qgs            Gate-Source charge storage                  |
     |qgd            Gate-Drain charge storage                   |
     |is             Source current                              |
     |                         continued                |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |     MES - instance output-only parameters - continued
     |-----------------------------------------------------------+
     | p                 Power dissipated by the mesfet          |
      -----------------------------------------------------------
      ------------------------------------------------------------
     |            MES - model parameters (input-only)            |
     |-----------------------------------------------------------+
     | nmf               N type MESfet model                     |
     | pmf               P type MESfet model                     |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |           MES - model parameters (input-output)           |
     |-----------------------------------------------------------+
     | vt0               Pinch-off voltage                       |
     | vto               (null)                                  |
     | alpha             Saturation voltage parameter            |
     | beta              Transconductance parameter              |
      ------------------------------------------------------------
     | lambda            Channel length modulation param.        |
     | b                 Doping tail extending parameter         |
     | rd                Drain ohmic resistance                  |
     | rs                Source ohmic resistance                 |
     |-----------------------------------------------------------+
     | cgs               G-S junction capacitance                |
     | cgd               G-D junction capacitance                |
     | pb                Gate junction potential                 |
     | is                Junction saturation current             |
      ------------------------------------------------------------
     | fc                Forward bias junction fit param.        |
     | kf                Flicker noise coefficient               |
     | af                Flicker noise exponent                  |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |            MES - model parameters (output-only)           |
     |-----------------------------------------------------------+
     | type              N-type or P-type MESfet model           |
     | gd                Drain conductance                       |
     | gs                Source conductance                      |
     | depl_cap          Depletion capacitance                   |
     | vcrit             Critical voltage                        |
      ------------------------------------------------------------


File: ngspice.info,  Node: Level 1 MOSfet model,  Next: Level 2 MOSfet model,  Prev: GaAs MESFET model,  Up: Model and Device Parameters

13.17 Mos1:  Level 1 MOSfet model with  Meyer capacitance model
===============================================================


      ------------------------------------------------------------
     |          Mos1 - instance parameters (input-only)          |
     |-----------------------------------------------------------+
     | off               Device initially off                    |
     | ic                Vector of D-S, G-S, B-S voltages        |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |         Mos1 - instance parameters (input-output)         |
     |-----------------------------------------------------------+
     | m                 Multiplicity
     | l                 Length                                  |
     | w                 Width                                   |
     | ad                Drain area                              |
     | as                Source area                             |
      ------------------------------------------------------------
     | pd                Drain perimeter                         |
     | ps                Source perimeter                        |
     | nrd               Drain squares                           |
     | nrs               Source squares                          |
     |-----------------------------------------------------------+
     | icvds             Initial D-S voltage                     |
     | icvgs             Initial G-S voltage                     |
     | icvbs             Initial B-S voltage                     |
     | temp              Instance temperature                    |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |          Mos1 - instance parameters (output-only)         |
     |-----------------------------------------------------------+
     | id                Drain current                           |
     | is                Source current                          |
     | ig                Gate current                            |
     | ib                Bulk current                            |
      ------------------------------------------------------------
     | ibd               B-D junction current                    |
     | ibs               B-S junction current                    |
     | vgs               Gate-Source voltage                     |
     | vds               Drain-Source voltage                    |
     |-----------------------------------------------------------+
     | vbs               Bulk-Source voltage                     |
     | vbd               Bulk-Drain voltage                      |
     | dnode             Number of the drain node                |
     | gnode             Number of the gate node                 |
      ------------------------------------------------------------
     | snode             Number of the source node               |
     | bnode             Number of the node                      |
     | dnodeprime        Number of int. drain node               |
     | snodeprime        Number of int. source node              |
     |-----------------------------------------------------------+
     | von                                                       |
     | vdsat             Saturation drain voltage                |
     | sourcevcrit       Critical source voltage                 |
     | drainvcrit        Critical drain voltage                  |
     | rs                Source resistance                       |
     |                         continued                         |
      ------------------------------------------------------------


      --------------------------------------------------------------
     |      Mos1 - instance output-only parameters - continued
     |-------------------------------------------------------------+
     |sourceconductanceConductance of source                       |
     |rd               Drain conductance                           |
     |drainconductance Conductance of drain                        |
     |gm               Transconductance                            |
      --------------------------------------------------------------
     |gds              Drain-Source conductance                    |
     |gmb              Bulk-Source transconductance                |
     |gmbs                                                         |
     |gbd              Bulk-Drain conductance                      |
     |-------------------------------------------------------------+
     |gbs              Bulk-Source conductance                     |
     |cbd              Bulk-Drain capacitance                      |
     |cbs              Bulk-Source capacitance                     |
     |cgs              Gate-Source capacitance                     |
      --------------------------------------------------------------
     |cgd              Gate-Drain capacitance                      |
     |cgb              Gate-Bulk capacitance                       |
     |cqgs             Capacitance due to gate-source charge storage
     |cqgd             Capacitance due to gate-drain charge storage|
     |-------------------------------------------------------------+
     |cqgb             Capacitance due to gate-bulk charge storage |
     |cqbd             Capacitance due to bulk-drain charge storage|
      cqbs             Capacitance due to bulk-source charge storage
     |cbd0             Zero-Bias B-D junction capacitance          |
      --------------------------------------------------------------
     |cbdsw0                                                       |
     |cbs0             Zero-Bias B-S junction capacitance          |
     |cbssw0                                                       |
     |qgs              Gate-Source charge storage                  |
     |-------------------------------------------------------------+
     |qgd              Gate-Drain charge storage                   |
     |qgb              Gate-Bulk charge storage                    |
     |qbd              Bulk-Drain charge storage                   |
     |qbs              Bulk-Source charge storage                  |
     |p                Instaneous power                            |
      --------------------------------------------------------------


      ------------------------------------------------------------
     |            Mos1 - model parameters (input-only)           |
     |-----------------------------------------------------------+
     | nmos              N type MOSfet model                     |
     | pmos              P type MOSfet model                     |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |           Mos1 - model parameters (input-output)          |
     |-----------------------------------------------------------+
     | vto               Threshold voltage                       |
     | vt0               (null)                                  |
     | kp                Transconductance parameter              |
     | gamma             Bulk threshold parameter                |
      ------------------------------------------------------------
     | phi               Surface potential                       |
     | lambda            Channel length modulation               |
     | rd                Drain ohmic resistance                  |
     |                         continued                         |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |      Mos1 - model input-output parameters - continued
     |-----------------------------------------------------------+
     | rs                Source ohmic resistance                 |
     | cbd               B-D junction capacitance                |
     | cbs               B-S junction capacitance                |
     | is                Bulk junction sat. current              |
      ------------------------------------------------------------
     | pb                Bulk junction potential                 |
     | cgso              Gate-source overlap cap.                |
     | cgdo              Gate-drain overlap cap.                 |
     | cgbo              Gate-bulk overlap cap.                  |
     |-----------------------------------------------------------+
     | rsh               Sheet resistance                        |
     | cj                Bottom junction cap per area            |
     | mj                Bottom grading coefficient              |
     | cjsw              Side junction cap per area              |
      ------------------------------------------------------------
     | mjsw              Side grading coefficient                |
     | js                Bulk jct. sat. current density          |
     | tox               Oxide thickness                         |
     | ld                Lateral diffusion                       |
     |-----------------------------------------------------------+
     | u0                Surface mobility                        |
     | uo                (null)                                  |
     | fc                Forward bias jct. fit param.           |
     | nsub              Substrate doping                        |
      ------------------------------------------------------------
     | tpg               Gate type                               |
     | nss               Surface state density                   |
     | tnom              Parameter measurement temperature       |
     | kf                Flicker noise coefficient               |
     | af                Flicker noise exponent                  |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |           Mos1 - model parameters (output-only)           |
     |-----------------------------------------------------------+
     | type              N-channel or P-channel MOS              |
      ------------------------------------------------------------


File: ngspice.info,  Node: Level 2 MOSfet model,  Next: Level 3 MOSfet model,  Prev: Level 1 MOSfet model,  Up: Model and Device Parameters

13.18 Mos2:  Level 2 MOSfet model with Meyer capacitance model
==============================================================


      ------------------------------------------------------------
     |          Mos2 - instance parameters (input-only)          |
     |-----------------------------------------------------------+
     | off               Device initially off                    |
     | ic                Vector of D-S, G-S, B-S voltages        |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |         Mos2 - instance parameters (input-output)         |
     |-----------------------------------------------------------+
     | m                 Multiplicity                            |
     | l                 Length                                  |
     | w                 Width                                   |
     | ad                Drain area                              |
     | as                Source area                             |
      ------------------------------------------------------------
     | pd                Drain perimeter                         |
     | ps                Source perimeter                        |
     | nrd               Drain squares                           |
     | nrs               Source squares                          |
     |-----------------------------------------------------------+
     | icvds             Initial D-S voltage                     |
     | icvgs             Initial G-S voltage                     |
     | icvbs             Initial B-S voltage                     |
     | temp              Instance operating temperature          |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |          Mos2 - instance parameters (output-only)         |
     |-----------------------------------------------------------+
     | id                Drain current                           |
     | cd                                                        |
     | ibd               B-D junction current                    |
     | ibs               B-S junction current                    |
      ------------------------------------------------------------
     | is                Source current                          |
     | ig                Gate current                            |
     | ib                Bulk current                            |
     | vgs               Gate-Source voltage                     |
     |-----------------------------------------------------------+
     | vds               Drain-Source voltage                    |
     | vbs               Bulk-Source voltage                     |
     | vbd               Bulk-Drain voltage                      |
     | dnode             Number of drain node                    |
      ------------------------------------------------------------
     | gnode             Number of gate node                     |
     | snode             Number of source node                   |
     | bnode             Number of bulk node                     |
     | dnodeprime        Number of internal drain node           |
     |-----------------------------------------------------------+
     | snodeprime        Number of internal source node          |
     | von                                                       |
     | vdsat             Saturation drain voltage                |
     | sourcevcrit       Critical source voltage                 |
     | drainvcrit        Critical drain voltage                  |
     |                         continued                         |
      ------------------------------------------------------------


      --------------------------------------------------------------
     |      Mos2 - instance output-only parameters - continued
     |-------------------------------------------------------------+
     |rs               Source resistance                           |
     |sourceconductanceSource conductance                          |
     |rd               Drain resistance                            |
     |drainconductance Drain conductance                           |
      --------------------------------------------------------------
     |gm               Transconductance                            |
     |gds              Drain-Source conductance                    |
     |gmb              Bulk-Source transconductance                |
     |gmbs                                                         |
     |-------------------------------------------------------------+
     |gbd              Bulk-Drain conductance                      |
     |gbs              Bulk-Source conductance                     |
     |cbd              Bulk-Drain capacitance                      |
     |cbs              Bulk-Source capacitance                     |
      --------------------------------------------------------------
     |cgs              Gate-Source capacitance                     |
     |cgd              Gate-Drain capacitance                      |
     |cgb              Gate-Bulk capacitance                       |
     |cbd0             Zero-Bias B-D junction capacitance          |
     |-------------------------------------------------------------+
     |cbdsw0                                                       |
     |cbs0             Zero-Bias B-S junction capacitance          |
     |cbssw0                                                       |
      cqgs             Capacitance due to gate-source charge storage
     |                                                             |
      --------------------------------------------------------------
     |cqgd             Capacitance due to gate-drain charge storage|
     |cqgb             Capacitance due to gate-bulk charge storage |
     |cqbd             Capacitance due to bulk-drain charge storage|
     |cqbs             Capacitance due to bulk-source charge storage
     |-------------------------------------------------------------+
     |qgs              Gate-Source charge storage                  |
     |qgd              Gate-Drain charge storage                   |
     |qgb              Gate-Bulk charge storage                    |
     |qbd              Bulk-Drain charge storage                   |
     |qbs              Bulk-Source charge storage                  |
     |p                Instantaneous power                         |
      --------------------------------------------------------------


      ------------------------------------------------------------
     |            Mos2 - model parameters (input-only)           |
     |-----------------------------------------------------------+
     | nmos              N type MOSfet model                     |
     | pmos              P type MOSfet model                     |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |           Mos2 - model parameters (input-output)          |
     |-----------------------------------------------------------+
     | vto               Threshold voltage                       |
     | vt0               (null)                                  |
     | kp                Transconductance parameter              |
     | gamma             Bulk threshold parameter                |
      ------------------------------------------------------------
     | phi               Surface potential                       |
     | lambda            Channel length modulation               |
     | rd                Drain ohmic resistance                  |
     | rs                Source ohmic resistance                 |
     |-----------------------------------------------------------+
     | cbd               B-D junction capacitance                |
     | cbs               B-S junction capacitance                |
     | is                Bulk junction sat. current              |
     | pb                Bulk junction potential                 |
      ------------------------------------------------------------
     | cgso              Gate-source overlap cap.                |
     | cgdo              Gate-drain overlap cap.                 |
     | cgbo              Gate-bulk overlap cap.                  |
     | rsh               Sheet resistance                        |
     |-----------------------------------------------------------+
     | cj                Bottom junction cap per area            |
     | mj                Bottom grading coefficient              |
     | cjsw              Side junction cap per area              |
     | mjsw              Side grading coefficient                |
      ------------------------------------------------------------
     | js                Bulk jct. sat. current density          |
     | tox               Oxide thickness                         |
     | ld                Lateral diffusion                       |
     | u0                Surface mobility                        |
     |-----------------------------------------------------------+
     | uo                (null)                                  |
     | fc                Forward bias jct. fit param.            |
     | nsub              Substrate doping                        |
     | tpg               Gate type                               |
      ------------------------------------------------------------
     | nss               Surface state density                   |
     | delta             Width effect on threshold               |
     | uexp              Crit. field exp for mob. deg.           |
     | ucrit             Crit. field for mob. degradation        |
     |-----------------------------------------------------------+
     | vmax              Maximum carrier drift velocity          |
     | xj                Junction depth                          |
     | neff              Total channel charge coeff.             |
     | nfs               Fast surface state density              |
      ------------------------------------------------------------
     | tnom              Parameter measurement temperature       |
     | kf                Flicker noise coefficient               |
     | af                Flicker noise exponent                  |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |           Mos2 - model parameters (output-only)           |
     |-----------------------------------------------------------+
     | type              N-channel or P-channel MOS              |
      ------------------------------------------------------------


File: ngspice.info,  Node: Level 3 MOSfet model,  Next: Level 6 MOSfet model,  Prev: Level 2 MOSfet model,  Up: Model and Device Parameters

13.19 Mos3: Level 3 MOSfet model with Meyer capacitance model
=============================================================



      ------------------------------------------------------------
     |          Mos3 - instance parameters (input-only)          |
     |-----------------------------------------------------------+
     | off               Device initially off                    |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |         Mos3 - instance parameters (input-output)         |
     |-----------------------------------------------------------+
     | m                 Multiplicity                            |
     | l                 Length                                  |
     | w                 Width                                   |
     | ad                Drain area                              |
     | as                Source area                             |
     ------------------------------------------------------------+
     | pd                Drain perimeter                         |
     | ps                Source perimeter                        |
     | nrd               Drain squares                           |
     | nrs               Source squares                          |
     |-----------------------------------------------------------+
     | icvds             Initial D-S voltage                     |
     | icvgs             Initial G-S voltage                     |
     | icvbs             Initial B-S voltage                     |
     | ic                Vector of D-S, G-S, B-S voltages        |
     | temp              Instance operating temperature          |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |          Mos3 - instance parameters (output-only)         |
     |-----------------------------------------------------------+
     | id                Drain current                           |
     | cd                Drain current                           |
     | ibd               B-D junction current                    |
     | ibs               B-S junction current                    |
      ------------------------------------------------------------
     | is                Source current                          |
     | ig                Gate current                            |
     | ib                Bulk current                            |
     | vgs               Gate-Source voltage                     |
     |-----------------------------------------------------------+
     | vds               Drain-Source voltage                    |
     | vbs               Bulk-Source voltage                     |
     | vbd               Bulk-Drain voltage                      |
     | dnode             Number of drain node                    |
      ------------------------------------------------------------
     | gnode             Number of gate node                     |
     | snode             Number of source node                   |
     | bnode             Number of bulk node                     |
     | dnodeprime        Number of internal drain node           |
     | snodeprime        Number of internal source node          |
     |                         continued                         |
      ------------------------------------------------------------


      --------------------------------------------------------------
     |      Mos3 - instance output-only parameters - continued
     |-------------------------------------------------------------+
     |von              Turn-on voltage                             |
     |vdsat            Saturation drain voltage                    |
     |sourcevcrit      Critical source voltage                     |
     |drainvcrit       Critical drain voltage                      |
      --------------------------------------------------------------
     |rs               Source resistance                           |
     |sourceconductanceSource conductance                          |
     |rd               Drain resistance                            |
     |drainconductance Drain conductance                           |
     |-------------------------------------------------------------+
     |gm               Transconductance                            |
     |gds              Drain-Source conductance                    |
     |gmb              Bulk-Source transconductance                |
     |gmbs             Bulk-Source transconductance                |
      --------------------------------------------------------------
     |gbd              Bulk-Drain conductance                      |
     |gbs              Bulk-Source conductance                     |
     |cbd              Bulk-Drain capacitance                      |
     |cbs              Bulk-Source capacitance                     |
     |-------------------------------------------------------------+
     |cgs              Gate-Source capacitance                     |
     |cgd              Gate-Drain capacitance                      |
     |cgb              Gate-Bulk capacitance                       |
      cqgs             Capacitance due to gate-source charge storage
     |                                                             |
      --------------------------------------------------------------
     |cqgd             Capacitance due to gate-drain charge storage|
     |cqgb             Capacitance due to gate-bulk charge storage |
     |cqbd             Capacitance due to bulk-drain charge storage|
     |cqbs             Capacitance due to bulk-source charge storage
     |-------------------------------------------------------------+
     |cbd0             Zero-Bias B-D junction capacitance          |
     |cbdsw0           Zero-Bias B-D sidewall capacitance          |
     |cbs0             Zero-Bias B-S junction capacitance          |
     |cbssw0           Zero-Bias B-S sidewall capacitance          |
      --------------------------------------------------------------
     |qbs              Bulk-Source charge storage                  |
     |qgs              Gate-Source charge storage                  |
     |qgd              Gate-Drain charge storage                   |
     |qgb              Gate-Bulk charge storage                    |
     |qbd              Bulk-Drain charge storage                   |
     |p                Instantaneous power                         |
      --------------------------------------------------------------


      ------------------------------------------------------------
     |            Mos3 - model parameters (input-only)           |
     |-----------------------------------------------------------+
     | nmos              N type MOSfet model                     |
     | pmos              P type MOSfet model                     |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |           Mos3 - model parameters (input-output)          |
     |-----------------------------------------------------------+
     | vto               Threshold voltage                       |
     | vt0               (null)                                  |
     | kp                Transconductance parameter              |
     | gamma             Bulk threshold parameter                |
      ------------------------------------------------------------
     | phi               Surface potential                       |
     | rd                Drain ohmic resistance                  |
     | rs                Source ohmic resistance                 |
     | cbd               B-D junction capacitance                |
     |-----------------------------------------------------------+
     | cbs               B-S junction capacitance                |
     | is                Bulk junction sat. current              |
     | pb                Bulk junction potential                 |
     | cgso              Gate-source overlap cap.                |
      ------------------------------------------------------------
     | cgdo              Gate-drain overlap cap.                 |
     | cgbo              Gate-bulk overlap cap.                  |
     | rsh               Sheet resistance                        |
     | cj                Bottom junction cap per area            |
     |-----------------------------------------------------------+
     | mj                Bottom grading coefficient              |
     | cjsw              Side junction cap per area              |
     | mjsw              Side grading coefficient                |
     | js                Bulk jct. sat. current density          |
      ------------------------------------------------------------
     | tox               Oxide thickness                         |
     | xl                Length mask adjustment                  |
     | wd                Width Narrowing (Diffusion)             |
     | xw                Width mask adjustment                   |
     | ld                Lateral diffusion                       |
     | u0                Surface mobility                        |
     | uo                (null)                                  |
     |-----------------------------------------------------------+
     | fc                Forward bias jct. fit param.            |
     | nsub              Substrate doping                        |
     | tpg               Gate type                               |
     | nss               Surface state density                   |
      ------------------------------------------------------------
     | vmax              Maximum carrier drift velocity          |
     | xj                Junction depth                          |
     | nfs               Fast surface state density              |
     | xd                Depletion layer width                   |
     |-----------------------------------------------------------+
     | alpha             Alpha                                   |
     | eta               Vds dependence of threshold voltage     |
     | delta             Width effect on threshold               |
     | input_delta       (null)                                  |
      ------------------------------------------------------------
     | theta             Vgs dependence on mobility              |
     | kappa             Kappa                                   |
     | tnom              Parameter measurement temperature       |
     | kf                Flicker noise coefficient               |
     | af                Flicker noise exponent                  |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |           Mos3 - model parameters (output-only)           |
     |-----------------------------------------------------------+
     | type              N-channel or P-channel MOS              |
      ------------------------------------------------------------


File: ngspice.info,  Node: Level 6 MOSfet model,  Next: Simple linear resistor,  Prev: Level 3 MOSfet model,  Up: Model and Device Parameters

13.20 Mos6: Level 6 MOSfet model with Meyer capacitance model
=============================================================



      ------------------------------------------------------------
     |          Mos6 - instance parameters (input-only)          |
     |-----------------------------------------------------------+
     | off               Device initially off                    |
     | ic                Vector of D-S, G-S, B-S voltages        |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |         Mos6 - instance parameters (input-output)         |
     |-----------------------------------------------------------+
     | l                 Length                                  |
     | w                 Width                                   |
     | ad                Drain area                              |
     | as                Source area                             |
      ------------------------------------------------------------
     | pd                Drain perimeter                         |
     | ps                Source perimeter                        |
     | nrd               Drain squares                           |
     | nrs               Source squares                          |
     |-----------------------------------------------------------+
     | icvds             Initial D-S voltage                     |
     | icvgs             Initial G-S voltage                     |
     | icvbs             Initial B-S voltage                     |
     | temp              Instance temperature                    |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |          Mos6 - instance parameters (output-only)         |
     |-----------------------------------------------------------+
     | id                Drain current                           |
     | cd                Drain current                           |
     | is                Source current                          |
     | ig                Gate current                            |
      ------------------------------------------------------------
     | ib                Bulk current                            |
     | ibs               B-S junction capacitance                |
     | ibd               B-D junction capacitance                |
     | vgs               Gate-Source voltage                     |
     |-----------------------------------------------------------+
     | vds               Drain-Source voltage                    |
     | vbs               Bulk-Source voltage                     |
     | vbd               Bulk-Drain voltage                      |
     | dnode             Number of the drain node                |
      ------------------------------------------------------------
     | gnode             Number of the gate node                 |
     | snode             Number of the source node               |
     | bnode             Number of the node                      |
     | dnodeprime        Number of int. drain node               |
     | snodeprime        Number of int. source node              |
     |                         continued                         |
      ------------------------------------------------------------


      --------------------------------------------------------------
     |      Mos6 - instance output-only parameters - continued
     |-------------------------------------------------------------+
     |rs               Source resistance                           |
     |sourceconductanceSource conductance                          |
     |rd               Drain resistance                            |
     |drainconductance Drain conductance                           |
      --------------------------------------------------------------
     |von              Turn-on voltage                             |
     |vdsat            Saturation drain voltage                    |
     |sourcevcrit      Critical source voltage                     |
     |drainvcrit       Critical drain voltage                      |
     |-------------------------------------------------------------+
     |gmbs             Bulk-Source transconductance                |
     |gm               Transconductance                            |
     |gds              Drain-Source conductance                    |
     |gbd              Bulk-Drain conductance                      |
      --------------------------------------------------------------
     |gbs              Bulk-Source conductance                     |
     |cgs              Gate-Source capacitance                     |
     |cgd              Gate-Drain capacitance                      |
     |cgb              Gate-Bulk capacitance                       |
     |-------------------------------------------------------------+
     |cbd              Bulk-Drain capacitance                      |
     |cbs              Bulk-Source capacitance                     |
     |cbd0             Zero-Bias B-D junction capacitance          |
     |cbdsw0                                                       |
      --------------------------------------------------------------
     |cbs0             Zero-Bias B-S junction capacitance          |
     |cbssw0                                                       |
     |cqgs             Capacitance due to gate-source charge storage
     |cqgd             Capacitance due to gate-drain charge storage|
     |-------------------------------------------------------------+
     |cqgb             Capacitance due to gate-bulk charge storage |
     |cqbd             Capacitance due to bulk-drain charge storage|
      cqbs             Capacitance due to bulk-source charge storage
     |qgs              Gate-Source charge storage                  |
      --------------------------------------------------------------
     |qgd              Gate-Drain charge storage                   |
     |qgb              Gate-Bulk charge storage                    |
     |qbd              Bulk-Drain charge storage                   |
     |qbs              Bulk-Source charge storage                  |
     |p                Instantaneous power                         |
      --------------------------------------------------------------


      ------------------------------------------------------------
     |            Mos6 - model parameters (input-only)           |
     |-----------------------------------------------------------+
     | nmos              N type MOSfet model                     |
     | pmos              P type MOSfet model                     |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |           Mos6 - model parameters (input-output)          |
     |-----------------------------------------------------------+
     | vto               Threshold voltage                       |
     | vt0               (null)                                  |
     | kv                Saturation voltage factor               |
     | nv                Saturation voltage coeff.               |
      ------------------------------------------------------------
     | kc                Saturation current factor               |
     | nc                Saturation current coeff.               |
     | nvth              Threshold voltage coeff.                |
     | ps                Sat. current modification  par.         |
     |-----------------------------------------------------------+
     | gamma             Bulk threshold parameter                |
     | gamma1            Bulk threshold parameter 1              |
     | sigma             Static feedback effect par.             |
     | phi               Surface potential                       |
      ------------------------------------------------------------
     | lambda            Channel length modulation param.        |
     | lambda0           Channel length modulation param. 0      |
     | lambda1           Channel length modulation param. 1      |
     | rd                Drain ohmic resistance                  |
     |-----------------------------------------------------------+
     | rs                Source ohmic resistance                 |
     | cbd               B-D junction capacitance                |
     | cbs               B-S junction capacitance                |
     | is                Bulk junction sat. current              |
      ------------------------------------------------------------
     | pb                Bulk junction potential                 |
     | cgso              Gate-source overlap cap.                |
     | cgdo              Gate-drain overlap cap.                 |
     | cgbo              Gate-bulk overlap cap.                  |
     |-----------------------------------------------------------+
     | rsh               Sheet resistance                        |
     | cj                Bottom junction cap per area            |
     | mj                Bottom grading coefficient              |
     | cjsw              Side junction cap per area              |
      ------------------------------------------------------------
     | mjsw              Side grading coefficient                |
     | js                Bulk jct. sat. current density          |
     | ld                Lateral diffusion                       |
     | tox               Oxide thickness                         |
     |-----------------------------------------------------------+
     | u0                Surface mobility                        |
     | uo                (null)                                  |
     | fc                Forward bias jct. fit param.            |
     | tpg               Gate type                               |
      ------------------------------------------------------------
     | nsub              Substrate doping                        |
     | nss               Surface state density                   |
     | tnom              Parameter measurement temperature       |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |           Mos6 - model parameters (output-only)           |
     |-----------------------------------------------------------+
     | type              N-channel or P-channel MOS              |
      ------------------------------------------------------------


File: ngspice.info,  Node: Simple linear resistor,  Next: Ideal voltage controlled switch,  Prev: Level 6 MOSfet model,  Up: Model and Device Parameters

13.21 Resistor:  Simple linear resistor
=======================================


      ------------------------------------------------------------
     |       Resistor - instance parameters (input-output)       |
     |-----------------------------------------------------------+
     | resistance        Resistance                              |
     | temp              Instance operating temperature          |
     | l                 Length                                  |
     | w                 Width                                   |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |        Resistor - instance parameters (output-only)       |
     |-----------------------------------------------------------+
     | i                 Current                                 |
     | p                 Power                                   |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |          Resistor - model parameters (input-only)         |
     |-----------------------------------------------------------+
     | r                 Device is a resistor model              |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |         Resistor - model parameters (input-output)        |
     |-----------------------------------------------------------+
     | rsh               Sheet resistance                        |
     | narrow            Narrowing of resistor                   |
     | tc1               First order temp. coefficient           |
     | tc2               Second order temp. coefficient          |
     | defw              Default device width                    |
     | tnom              Parameter measurement temperature       |
      ------------------------------------------------------------


File: ngspice.info,  Node: Ideal voltage controlled switch,  Next: Lossless transmission line,  Prev: Simple linear resistor,  Up: Model and Device Parameters

13.22 Switch:  Ideal voltage controlled switch
==============================================


      ------------------------------------------------------------
     |         Switch - instance parameters (input-only)         |
     |-----------------------------------------------------------+
     | on                Switch initially closed                 |
     | off               Switch initially open                   |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |        Switch - instance parameters (input-output)        |
     |-----------------------------------------------------------+
     | pos_node          Positive node of switch                 |
     | neg_node          Negative node of switch                 |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |         Switch - instance parameters (output-only)        |
     |-----------------------------------------------------------+
     | cont_p_node       Positive contr. node of switch          |
     | cont_n_node       Positive contr. node of switch          |
     | i                 Switch current                          |
     | p                 Switch power                            |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |          Switch - model parameters (input-output)         |
     |-----------------------------------------------------------+
     | sw                Switch model                            |
     | vt                Threshold voltage                       |
     | vh                Hysteresis voltage                      |
     | ron               Resistance when closed                  |
     | roff              Resistance when open                    |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |          Switch - model parameters (output-only)          |
     |-----------------------------------------------------------+
     | gon               Conductance when closed                 |
     | goff              Conductance when open                   |
      ------------------------------------------------------------


File: ngspice.info,  Node: Lossless transmission line,  Next: Voltage controlled current source,  Prev: Ideal voltage controlled switch,  Up: Model and Device Parameters

13.23 Tranline:  Lossless transmission line
===========================================


      ------------------------------------------------------------
     |        Tranline - instance parameters (input-only)        |
     |-----------------------------------------------------------+
     | ic                Initial condition vector:v1,i1,v2,i2    |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |       Tranline - instance parameters (input-output)       |
     |-----------------------------------------------------------+
     | z0                Characteristic impedance                |
     | zo                (null)                                  |
     | f                 Frequency                               |
     | td                Transmission delay                      |
      ------------------------------------------------------------
     | nl                Normalized length at frequency given    |
     | v1                Initial voltage at end 1                |
     | v2                Initial voltage at end 2                |
     | i1                Initial current at end 1                |
     | i2                Initial current at end 2                |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |        Tranline - instance parameters (output-only)       |
     |-----------------------------------------------------------+
     | rel               Rel. rate of change of deriv. for bkpt  |
     | abs               Abs. rate of change of deriv. for bkpt  |
     | pos_node1         Positive node of end 1 of t. line       |
     | neg_node1         Negative node of end 1 of t. line       |
      ------------------------------------------------------------
     | pos_node2         Positive node of end 2 of t. line       |
     | neg_node2         Negative node of end 2 of t. line       |
     | delays            Delayed values of excitation            |
      ------------------------------------------------------------


File: ngspice.info,  Node: Voltage controlled current source,  Next: Voltage controlled voltage source,  Prev: Lossless transmission line,  Up: Model and Device Parameters

13.24 VCCS:  Voltage controlled current source
==============================================


      ------------------------------------------------------------
     |          VCCS - instance parameters (input-only)          |
     |-----------------------------------------------------------+
     | ic                Initial condition of controlling source |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |         VCCS - instance parameters (input-output)         |
     |-----------------------------------------------------------+
     | gain              Transconductance of source (gain)       |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |          VCCS - instance parameters (output-only)         |
     |-----------------------------------------------------------+
     | pos_node          Positive node of source                 |
     | neg_node          Negative node of source                 |
     | cont_p_node       Positive node of contr. source          |
     | cont_n_node       Negative node of contr. source          |
      ------------------------------------------------------------
     | i                 Output current                          |
     | v                 Voltage across output                   |
     | p                 Power                                   |
      ------------------------------------------------------------


File: ngspice.info,  Node: Voltage controlled voltage source,  Next: Independent voltage source,  Prev: Voltage controlled current source,  Up: Model and Device Parameters

13.25 VCVS:  Voltage controlled voltage source
==============================================


      ------------------------------------------------------------
     |          VCVS - instance parameters (input-only)          |
     |-----------------------------------------------------------+
     | ic                Initial condition of controlling source |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |         VCVS - instance parameters (input-output)         |
     |-----------------------------------------------------------+
     | gain              Voltage gain                            |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |          VCVS - instance parameters (output-only)         |
     |-----------------------------------------------------------+
     | pos_node          Positive node of source                 |
     | neg_node          Negative node of source                 |
     | cont_p_node       Positive node of contr. source          |
       cont_n_node       Negative node of contr. source
      ------------------------------------------------------------
     | i                 Output current                          |
     | v                 Output voltage                          |
     | p                 Power                                   |
      ------------------------------------------------------------


File: ngspice.info,  Node: Independent voltage source,  Prev: Voltage controlled voltage source,  Up: Model and Device Parameters

13.26 Vsource:  Independent voltage source
==========================================


      ------------------------------------------------------------
     |         Vsource - instance parameters (input-only)        |
     |-----------------------------------------------------------+
     | pulse             Pulse description                       |
     | sine              Sinusoidal source description           |
     | sin               Sinusoidal source description           |
     | exp               Exponential source description          |
      ------------------------------------------------------------
     | pwl               Piecewise linear description            |
     | sffm              Single freq. FM description             |
     | ac                AC magnitude, phase vector              |
     | distof1           f1 input for distortion                 |
     | distof2           f2 input for distortion                 |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |        Vsource - instance parameters (input-output)       |
     |-----------------------------------------------------------+
     | dc                D.C. source value                       |
     | acmag             A.C. Magnitude                          |
     | acphase           A.C. Phase                              |
      ------------------------------------------------------------


      ------------------------------------------------------------
     |        Vsource - instance parameters (output-only)        |
     |-----------------------------------------------------------+
     | pos_node          Positive node of source                 |
     | neg_node          Negative node of source                 |
     | function          Function of the source                  |
     | order             Order of the source function            |
      ------------------------------------------------------------
     | coeffs            Coefficients for the function           |
     | acreal            AC real part                            |
     | acimag            AC imaginary part                       |
     | i                 Voltage source current                  |
     | p                 Instantaneous power                     |
      ------------------------------------------------------------

14 NGSPICE enhancements over Spice3
***********************************

NGSPICE is the result of many hours of work spent in front of a screen
trying to fix and enhance the original Spice3 code. Most of the work
done affects simulation results in some way, so many users ask why the
results obtained with Spice3 differ with the ones they get from NGSPICE.

   This chapter collects all the enhancements introduced into NGSPICE
during its development, ordered by categories. For each improvement
described here, the file(s) and function(s) affected are reported into
a table, letting the experienced user to understand at what extent such
improvement affects his or her simulation.

14.1 Device models code
=======================

This section collects most of the enhancements made to the code that
builds up device models and device support routines. If you are
concerned about discrepancies between the results you get with NGSPICE
and the ones you got with a clean Spice3f, look here to see if they
depend on a bug that has been fixed (or a new on introduced)

14.1.1 Resistor Model
---------------------

The NGSPICE resistor model has been enhanced adding some useful
features already present in other simulators:

   * Different resistance value for AC analysis (Serban Popescu).

   * Device Multiplicity. The "M" parameter simulates "M" paralleled
       resistors (Serban Popescu).

   * "Short" model parameter to take into account resistor shortening
        due to side etching. The original spice3 implementation had
     only       the "narrow" parameter (Alan Gillespie).

   * "scale" instance parameter to scale the AC or DC value (Paolo
     Nenzi).


Authors:
     Alan Gillespie, Paolo Nenzi, Serban Popescu

File:
     `spicelib/dev/res/*'

Function:
     All the functions that makes up the model.

Affects:
     The resistor model only.

14.1.2 Capacitor Model
----------------------

In `CAPask()', the power stored in a capacitor and current through it
were not showed correctly during transient analysis.


Author:
     Alan Gillespie

File:
     `spicelib/devices/cap/capask.c'

Function:
     `CAPask()'

Affects:
     The capacitor model only.

14.1.3 Diode (D) model fixes
----------------------------

In the original implementation of the diode model, the parameter
`DIOtBrkdwnV' was used instead of the flag `DIObreakdownVoltageGiven',
in the `DIOload()' function. In the same function the `DIOjunctionPot'
was used instead of the temperature corrected version `DIOtJctPot'.

   In the `DIOtemp()' function, the `DIOtVcrit' was calculated without
taking into account the device area.  This could cause floating point
overflows, especially in device models designed to be scaled by a small
area, e.g. 2u by 2u diodes (area=4e-12).

   The flawed code was:

     here->DIOtVcrit=vte*log(vte/(CONSTroot2*here->DIOtSatCur));

     here->DIOtVcrit=vte*
            log(vte/(CONSTroot2*here->DIOtSatCur*here->DIOarea));

ENHANCEMENT DATA:

Author:
     Alan Gillespie

Files:
     `spicelib/devices/dioload.c' `spicelib/devices/diotemp.c'

Function:
     `DIOload(), DIOtemp()'

Affects:
     The pn junction diode model.

14.1.4 Level 1 MOS model
------------------------

The Level 1 MOS model (MOS1)now accepts the "M" device parameter
(multiplicity), to simulate "M" paralleled identical devices. The "M"
parameter affects the following quantities:

   * In the AC load routine (`MOS1acLoad()'), the value assigned to the
     "M" (`MOS1m') parameter multiplies the overlap capacitances:
     `GateSourceOverlapCap', `GateDrainOverlapCap',
     `GateBulkOverlapCap'.

   * In the instance parameters ask routine (`MOS1ask()'), the value of
     gate-source, gate-drain and gate-bulk capacitances, corresponding
     to the parameters: `MOS1_CAPGS', `MOS1_CAPGD', `MOS1_CAPGB', are
     multiplied by the value of "M".

   * In the distortion analysis setup routine (`MOS1dset()'), the
     overlap capcitances (`GateSourceOverlapCap',
     `GateDrainOverlapCap', `GateBulkOverlapCap'), the saturation
     currents (`DrainSatCurr', `SourceSatCurr'), the "beta" (`Beta')
     and the oxide capacitance (`OxideCap') are all mutiplied by the
     value of "M".

   * In the main load routine (`MOS1load()'), the value of "M" paramter
     multiplies:`DrainSatCurr', `SourceSatCurr',
     `GateSourceOverlapCap', `GateDrainOverlapCap',
     `GateBulkOverlapCap', `Beta', `OxideCap'. The meaning of the
     variables have been already explained above.

   * In the noise analysis routine (in `MOS1noi()'), the noise
     densities, contained in the `noizDEns[]' vector are multplied by
     the value of "M".

   * In the load routine for Pole-Zero analysis, the following
     quantities are multiplied by the value of "M":
     `GateSourceOverlapCap', `GateDrainOverlapCap',
     `GateBulkOverlapCap'.

   * In the device "temp" routine (in `MOS1temp()') the source and
     drain critical voltages (`MOS1sourceVcrit', `MOS1drainVcrit') are
     multiplied by the value of "M", like the zero-voltage bulk-drain
     and bulk-source capacitances: `czbd', `czbdsw', `czbs', `czbssw',
     where "sw" suffix stands for "sidewall" and means perimetral
     capacitsnces and the drain and sources conductances (
     `MOS1drainConductance'. `MOS1sourceConductance')

   Other minor changes for "M" parameter support includes: `MOS1sprt()'
prints the value of "M", `MOS1param()' sets the value of "M" and
`MOS1ask()' returns that value.

   The "Gmin" implementation across the substrate diodes of MOS1 was
incorrect, correcting this dramatically improved DC convergence. The
original code in `MOS1load()' was:

     ...
     ...
     next1:  if(vbs <= 0) {
                 here->MOS1gbs = SourceSatCur/vt;
                 here->MOS1cbs = here->MOS1gbs*vbs;
                 here->MOS1gbs += ckt->CKTgmin;
             } else {
                 evbs = exp(MIN(MAX_EXP_ARG,vbs/vt));
                 here->MOS1gbs = SourceSatCur*evbs/vt + ckt->CKTgmin;
                 here->MOS1cbs = SourceSatCur * (evbs-1);
             }
             if(vbd <= 0) {
                 here->MOS1gbd = DrainSatCur/vt;
                 here->MOS1cbd = here->MOS1gbd *vbd;
                 here->MOS1gbd += ckt->CKTgmin;
             } else {
                 evbd = exp(MIN(MAX_EXP_ARG,vbd/vt));
                 here->MOS1gbd = DrainSatCur*evbd/vt +ckt->CKTgmin;
                 here->MOS1cbd = DrainSatCur *(evbd-1);
             }
     ...
     ...

   and the new one is:
     ...
     ...
     next1:  if(vbs <= -3*vt) {
                here->MOS1gbs = ckt->CKTgmin;
                here->MOS1cbs = here->MOS1gbs*vbs-SourceSatCur;
             } else {
                evbs = exp(MIN(MAX_EXP_ARG,vbs/vt));
                here->MOS1gbs = SourceSatCur*evbs/vt + ckt->CKTgmin;
                here->MOS1cbs = SourceSatCur*(evbs-1) + ckt->CKTgmin*vbs;
             }
             if(vbd <= -3*vt) {
                 here->MOS1gbd = ckt->CKTgmin;
                 here->MOS1cbd = here->MOS1gbd*vbd-DrainSatCur;
             } else {
                 evbd = exp(MIN(MAX_EXP_ARG,vbd/vt));
                 here->MOS1gbd = DrainSatCur*evbd/vt + ckt->CKTgmin;
                 here->MOS1cbd = DrainSatCur*(evbd-1) + ckt->CKTgmin*vbd;
             }
     ...
     ...

   In the "load current vector" section of the `MOS1load()' routine,
"Gmin" appeared in the calculation of `ceqbd' and `ceqbs':

          /*
           *  load current vector
           */

           ceqbs = model->MOS1type *
                   (here->MOS1cbs-(here->MOS1gbs-ckt->CKTgmin)*vbs);
           ceqbd = model->MOS1type *
                   (here->MOS1cbd-(here->MOS1gbd-ckt->CKTgmin)*vbd);

   The code has been corrected as follows:

          /*
           *  load current vector
           */

           ceqbs = model->MOS1type *
                   (here->MOS1cbs-(here->MOS1gbs)*vbs);
           ceqbd = model->MOS1type *
                   (here->MOS1cbd-(here->MOS1gbd)*vbd);

   MOS1 device reported only half of the Meyer capcitance without
adding the overlap capacitance contribution, when reporting to the
`.OP' printout or in the rawfile. The routine `MOS1ask()' was
responsible for this:

     ...
     ...
      case MOS1_CGS:
           value->rValue = *(ckt->CKTstate0 + here->MOS1capgs);
           return(OK);
      case MOS1_CGD:
           value->rValue = *(ckt->CKTstate0 + here->MOS1capgd);
           return(OK);
     ...
     ...
      case MOS1_CAPGS:
           value->rValue = *(ckt->CKTstate0 + here->MOS1capgs);
           return(OK);
     ...
     ...
      case MOS1_CAPGD:
           value->rValue = *(ckt->CKTstate0 + here->MOS1capgd);
           return(OK);
     ...
     ...
      case MOS1_CAPGB:
           value->rValue = *(ckt->CKTstate0 + here->MOS1capgb);
           return(OK);

   The new code is:

     ...
     ...
      case MOS1_CGS:
           value->rValue = 2* *(ckt->CKTstate0 + here->MOS1capgs);
           return(OK);
      case MOS1_CGD:
           value->rValue = 2* *(ckt->CKTstate0 + here->MOS1capgd);
           return(OK);
     ...
     ...
      case MOS1_CAPGS:
         value->rValue = 2* *(ckt->CKTstate0 + here->MOS1capgs);
         /* add overlap capacitance */
         value->rValue += (here->sMOS1modPtr->MOS1gateSourceOverlapCapFactor)
                           * here->MOS1m
                           * (here->MOS1w);
           return(OK);
     ...
     ...
      case MOS1_CAPGD:
         value->rValue = 2* *(ckt->CKTstate0 + here->MOS1capgd);
         /* add overlap capacitance */
         value->rValue += (here->sMOS1modPtr->MOS1gateSourceOverlapCapFactor)
                           * here->MOS1m
                           * (here->MOS1w);
           return(OK);
     ...
     ...
      case MOS1_CAPGB:
         value->rValue = 2* *(ckt->CKTstate0 + here->MOS1capgb);
         /* add overlap capacitance */
         value->rValue += (here->sMOS1modPtr->MOS1gateBulkOverlapCapFactor)
                           * here->MOS1m
                           * (here->MOS1l
                           -2*(here->sMOS1modPtr->MOS1latDiff));
           return(OK);

14.1.5 Level 2 MOS Model
------------------------

Level 2 mosfet model now accetps the "M" instance parameter
(multiplicity) to simulate M paralleled identical devices. The affected
quantities are:

   * In the AC load routine (`MOS2acLoad()', the value assigned
     to the "M" (`MOS2m') parameter, multiplies the overlap
     capacitance: ` GateSourceOverlapCap', ` GateDrainOverlapCap',
     ` GateBulkOverlapCap'.

   * In the `MOS2ask()' routine (instance parameters reporting) the
      gate-source, gate-drain and gate-bulk capacitances, corresponding
          to `MOS2_CAPGS', `MOS2_CAPGD', `MOS2_CAPGB'
     parameters, are multiplied by the value of "M".

   * In the `MOS2dset()' function (distortion analysis setup)       the
     overlap capcitances (`GateSourceOverlapCap',
     `GateDrainOverlapCap', `GateBulkOverlapCap'),       the saturation
     currents (`DrainSatCurr', `SourceSatCurr'),       the "beta"
     (`Beta'), the oxide capacitance (`OxideCap')       and and the
     `xn' quantity are all mutiplied by the value       of "M".

   * In the main load routine `MOS2load()', the value of "M"
     parameter multiplies:`DrainSatCurr', `SourceSatCurr',
     `GateSourceOverlapCap', `GateDrainOverlapCap',
     `GateBulkOverlapCap', `Beta', `OxideCap',       `xn'. The meaning
     of the variables have been already       explained above.

   * In the noise analysis routine `MOS2noi()', the noise
     densities, contained in the `noizDEns[]' vector are
     multplied by the value of "M".

   * In the load routine for Pole-Zero analysis (`MOS2pzLoad()'),
     the following quantities are multiplied by the value of "M":
     `GateSourceOverlapCap', `GateDrainOverlapCap',
     `GateBulkOverlapCap'.

   * In `MOS2temp()' routine the source and drain critical
     voltages (`MOS2sourceVcrit', `MOS2drainVcrit')       are
     multiplied by the value of "M", like the zero-voltage
     bulk-drain and bulk-source capacitances: `czbd',       `czbdsw',
     `czbs', `czbssw', where "sw" suffix       stands for "sidewall"
     and means perimetral capacitances and       the drain and sources
     conductances (`MOS2drainConductance',
     `MOS2sourceConductance').

   Other minor changes for "M" parameter support includes: `MOS2sprt()'
prints the value of "M", `MOS2param()' sets the value of "M" and
`MOS2ask()' returns that value.

   The "Gmin" implementation across the substrate diodes of MOS2 was
incorrect, correcting this dramatically improved DC convergence. The
original code in `MOS2load()' was:

     ...
     ...
      /* bulk-source and bulk-drain diodes
       * here we just evaluate the ideal diode current and the
       * corresponding derivative (conductance).
       */

     next1:      if(vbs <= 0) {
                     here->MOS2gbs = SourceSatCur/vt;
                     here->MOS2cbs = here->MOS2gbs*vbs;
                     here->MOS2gbs += ckt->CKTgmin;
                 } else {
                     evbs = exp(vbs/vt);
                     here->MOS2gbs = SourceSatCur*evbs/vt + ckt->CKTgmin;
                     here->MOS2cbs = SourceSatCur * (evbs-1);
                 }
                 if(vbd <= 0) {
                     here->MOS2gbd = DrainSatCur/vt;
                     here->MOS2cbd = here->MOS2gbd *vbd;
                     here->MOS2gbd += ckt->CKTgmin;
                 } else {
                     evbd = exp(vbd/vt);
                     here->MOS2gbd = DrainSatCur*evbd/vt +ckt->CKTgmin;
                     here->MOS2cbd = DrainSatCur *(evbd-1);
                 }

     ...
     ...

   Then new code is:

     ...
     ...
      /* bulk-source and bulk-drain diodes
       * here we just evaluate the ideal diode current and the
       * corresponding derivative (conductance).
       */
     next1:    if(vbs <= -3*vt) {
                   here->MOS2gbs = ckt->CKTgmin;
                   here->MOS2cbs = here->MOS2gbs*vbs-SourceSatCur;
               } else {
                   evbs = exp(MIN(MAX_EXP_ARG,vbs/vt));
                   here->MOS2gbs = SourceSatCur*evbs/vt + ckt->CKTgmin;
                   here->MOS2cbs = SourceSatCur*(evbs-1) + ckt->CKTgmin*vbs;
               }
               if(vbd <= -3*vt) {
                   here->MOS2gbd = ckt->CKTgmin;
                   here->MOS2cbd = here->MOS2gbd*vbd-DrainSatCur;
               } else {
                   evbd = exp(MIN(MAX_EXP_ARG,vbd/vt));
                   here->MOS2gbd = DrainSatCur*evbd/vt + ckt->CKTgmin;
                   here->MOS2cbd = DrainSatCur*(evbd-1) + ckt->CKTgmin*vbd;
               }

   In the "load current vector" section of the `MOS2load()' routine,
"Gmin" appeared in the calculation of `ceqbd' and `ceqbs':

     ...
     ...
      /*
       *  load current vector
       */
          ceqbs = model->MOS2type *
                  (here->MOS2cbs-(here->MOS2gbs-ckt->CKTgmin)*vbs);
          ceqbd = model->MOS2type *
                  (here->MOS2cbd-(here->MOS2gbd-ckt->CKTgmin)*vbd);
     ...
     ...

   The correct code is:

     ...
     ...
      /*
       *  load current vector
       */
          ceqbs = model->MOS2type *
                  (here->MOS2cbs-(here->MOS2gbs)*vbs);
          ceqbd = model->MOS2type *
                  (here->MOS2cbd-(here->MOS2gbd)*vbd);
     ...
     ...

   MOS2 device reported only half of the Meyer capacitance without
adding the overlap capacitance contribution, when reporting to the
`.OP' printout or in the rawfile. The routine `MOS2ask()' was
responsible for this:

     ...
     ...
      case MOS2_CGS:
              value->rValue = *(ckt->CKTstate0 + here->MOS2capgs);
              return(OK);
      case MOS2_CGD:
              value->rValue = *(ckt->CKTstate0 + here->MOS2capgd);
              return(OK);
     ...
     ...
      case MOS2_CAPGS:
              value->rValue = *(ckt->CKTstate0 + here->MOS2capgs);
              return(OK);
     ...
     ...
      case MOS2_CAPGD:
              value->rValue = *(ckt->CKTstate0 + here->MOS2capgd);
              return(OK);
     ...
     ...
      case MOS2_CAPGB:
              value->rValue = *(ckt->CKTstate0 + here->MOS2capgb);
              return(OK);
     ...
     ...

   The new code is:

     ...
     ...
      case MOS2_CGS:
              value->rValue = 2* *(ckt->CKTstate0 + here->MOS2capgs);
              return(OK);
      case MOS2_CGD:
              value->rValue = 2* *(ckt->CKTstate0 + here->MOS2capgd);
              return(OK);
     ...
     ...
      case MOS2_CAPGS:
           value->rValue = 2* *(ckt->CKTstate0 + here->MOS2capgs);
           /* add overlap capacitance */
           value->rValue +=
               (here->MOS2modPtr->MOS2gateSourceOverlapCapFactor)
                * here->MOS2m
                * (here->MOS2w);
           return(OK);
     ...
     ...
      case MOS2_CAPGD:
           value->rValue = 2* *(ckt->CKTstate0 + here->MOS2capgd);
           /* add overlap capacitance */
           value->rValue +=
                (here->MOS2modPtr->MOS2gateSourceOverlapCapFactor)
                 * here->MOS2m
                 * (here->MOS2w);
           return(OK);
     ...
     ...
      case MOS2_CAPGB:
           value->rValue = 2* *(ckt->CKTstate0 + here->MOS2capgb);
           /* add overlap capacitance */
           value->rValue +=
                (here->MOS2modPtr->MOS2gateBulkOverlapCapFactor)
                 * here->MOS2m
                 * (here->MOS2l
                 -2*(here->MOS2modPtr->MOS2latDiff));
           return(OK);
     ...
     ...

   The level 2 MOSFET model seems to calculate Von and Vth values for
the threshold and subthreshold values respectively, but then uses Vbin
to calculate the Vdsat voltage used to find the drain current. However,
a jump statement uses Von to decide that the device is in the "cutoff"
region, which means that when this jump allows the drain current to be
calculated, Vdsat can already be well above zero. This leads to a
discontinuity of drain current with respect to gate voltage. The code
is now modified to use Vbin for the jump decision. It looks like the
code should actually use Vth as the threshold voltage, but since PSPICE
and HSPICE both follow the original Berkeley code, this was left alone.
The affected code can be found in `MOS2load()':

     ...
     ...
           if ((lvds-lvbs) >= 0) {
                barg = sqrt(phiMinVbs+lvds);
                dbrgdb = -0.5/barg;
     ...
     ...
                 vgst = lvgs-von;
                 if (lvgs <= von) {
                     /*
                      *  cutoff region
                      */
     ...
     ...
                 if (lvgs > von) goto line900;
                 /*
                  *  subthreshold region
                  */
     ...
     ...

   and the corrected code is:

     ...
     ...
           if ((lvbs-lvds) <= 0) {
                barg = sqrt(phiMinVbs+lvds);
                dbrgdb = -0.5/barg;
     ...
     ...

                 vgst = lvgs-von;
                 if (lvgs <= vbin) {
                     /*
                      *  cutoff region
                      */
     ...
     ...
                 if (model->MOS2fastSurfaceStateDensity != 0
                     && OxideCap != 0) {
                     if (lvgs > von) goto line900;
                 } else {
                     if (lvgs > vbin) goto line900;
                     goto doneval;
                 }
                 /*
                  *  subthreshold region
                  */
     ...
     ...

14.1.6 Level 3 Mos Model
------------------------

The level 3 model has been extensively corrected since it is a de-facto
standard for circuit simulation.

   The level 3 model supports the "M" parameter (multiplicity), which
can be used to simulate M identical paralleled devices. The "M"
parameter affects the quantities described in the following list:

   * In the AC load routine (`MOS3acld()', the value assigned       to
     the "M" (`MOS3m') parameter, multiplies the overlap
     capacitance: ` GateSourceOverlapCap', ` GateDrainOverlapCap',
     ` GateBulkOverlapCap'.

   * In the `MOS3ask()' function (instance parameters reporting) the
       gate-source, gate-drain and gate-bulk capacitances,
     corresponding       to `MOS3_CAPGS', `MOS3_CAPGD', `MOS3_CAPGB'
       parameters, are multiplied by the value of "M".

   * In the `MOS3dset()' function (distorsion analysis setup)       the
     overlap capcitances (`GateSourceOverlapCap',
     `GateDrainOverlapCap', `GateBulkOverlapCap'),       the saturation
     currents (`DrainSatCurr', `SourceSatCurr'),       the "beta"
     (`Beta'), the oxide capacitance (`OxideCap')       and and the
     `csonco' quantity are all mutiplied by the value       of "M".

   * In the main load routine `MOS3load()', the value of "M"
     parameter multiplies:`DrainSatCurr', `SourceSatCurr',
     `GateSourceOverlapCap', `GateDrainOverlapCap',
     `GateBulkOverlapCap', `Beta', `OxideCap',       `csonco'. The
     meaning of the variables have been already       explained above.

   * In the noise analysis routine `MOS3noi()', the noise
     densities, contained in the `noizDEns[]' vector are
     multplied by the value of "M".

   * In the load routine for Pole-Zero analysis (`MOS3pzLoad()'),
     the following quantities are multiplied by the value of "M":
     `GateSourceOverlapCap', `GateDrainOverlapCap',
     `GateBulkOverlapCap'.

   * In `MOS3temp()' routine the source and drain critical
     voltages (`MOS3sourceVcrit', `MOS3drainVcrit')       are
     multiplied by the value of "M", like the zero-voltage
     bulk-drain and bulk-source capacitances: `czbd',       `czbdsw',
     `czbs', `czbssw', where "sw" suffix       stands for "sidewall"
     and means perimetral capacitances and       the drain and sources
     conductances (`MOS3drainConductance',
     `MOS3sourceConductance').

   Other minor changes for "M" parameter support includes: `MOS3sprt()'
prints the value of "M", `MOS3param()' sets the value of "M" and
`MOS3ask()' returns that value.

   Another important improvement over the original Spice3 code is the
support for process narrowing over drawn dimensions. The three model
parameters added to level 3 model are: `xl', `wd', `xw'.  The changes
in the code are described in depth as a reference for future model
development.

   Adding new model parameters usually need the introduction of new
variables (one for each parameter) in the model structure:
`sMOS3model', which can be found in `mos3defs.h'. In this case the new
variables are:

     ...
     ...
     double MOS3lengthAdjust;    /* New param: mask adjustment to length */
     double MOS3widthNarrow;     /* New param to reduce effective width */
     double MOS3widthAdjust;     /* New param: mask adjustment to width */
     ...
     ...
     unsigned MOS3lengthAdjustGiven  :1;
     unsigned MOS3widthNarrowGiven   :1;
     unsigned MOS3widthAdjustGiven   :1;
     ...
     ...
     #define MOS3_MOD_XL 145
     #define MOS3_MOD_WD 146
     #define MOS3_MOD_XW 147
     ...
     ...

   The single bit field that ends in "Given" are used to indicate
whether the parameter has been supplied by the user or must be
defaulted.  The last three `#define' are needed as a mean to identify
the parameters throughout the model, since comparing integers is faster
than comparing stings. As you may have already imagined, those numbers
must be unique. The association between parameter name and numerical
code appears in `MOS3mPTable[]' in `mos3.c':

     ...
     ...
     IFparm MOS3mPTable[] = { /* model parameters */
      OP("type",   MOS3_MOD_TYPE,  IF_STRING ,"N-channel or P-channel MOS"),
      IP("nmos",   MOS3_MOD_NMOS,  IF_FLAG   ,"N type MOSfet model"),
      IP("pmos",   MOS3_MOD_PMOS,  IF_FLAG   ,"P type MOSfet model"),
     ...
     ...
      IOP("xl",    MOS3_MOD_XL,    IF_REAL   ,"Length mask adjustment"),
      IOP("wd",    MOS3_MOD_WD,    IF_REAL   ,"Width Narrowing (Diffusion)"),
      IOP("xw",    MOS3_MOD_XW,    IF_REAL   ,"Width mask adjustment"),
     ...
     ...

   The keyword `IOP' before the three parameters sets them as
input/output parameters (that can be set and queried). The function
used to set parameters values is `MOS3mParam()', which contains the
following code:

     ...
     ...
             case MOS3_MOD_XL:
                 model->MOS3lengthAdjust = value->rValue;
                 model->MOS3lengthAdjustGiven = TRUE;
                 break;
             case MOS3_MOD_WD:
                 model->MOS3widthNarrow = value->rValue;
                 model->MOS3widthNarrowGiven = TRUE;
                 break;
             case MOS3_MOD_XW:
                 model->MOS3widthAdjust = value->rValue;
                 model->MOS3widthAdjustGiven = TRUE;
                 break;
     ...
     ...

   The function used to query those parameters is `MOS3mAsk()' and the
specific code is:

     ...
     ...
             case MOS3_MOD_XL:
                 value->rValue = here->MOS3lengthAdjust;
                 return(OK);
             case MOS3_MOD_WD:
                 value->rValue = here->MOS3widthNarrow;
                 return(OK);
             case MOS3_MOD_XW:
                 value->rValue = here->MOS3widthAdjust;
                 return(OK);
     ...
     ...

   The code above describes the interface to the new parameters, their
influence on the model behaviour is contained in the following
functions: `MOS3acLoad()', `MOS3load()', `MOS3noise()', `MOS3pzLoad()',
`MOS3setup()', `MOS3sLoad()' and `MOS3temp()'.

   The `MOS3acLoad()' function contains the code used to represent the
model for AC (small signal) analysis. The original code was:

     ...
     ...
             EffectiveLength=here->MOS3l - 2*model->MOS3latDiff;
             GateSourceOverlapCap = model->MOS3gateSourceOverlapCapFactor *
                     here->MOS3w;
             GateDrainOverlapCap = model->MOS3gateDrainOverlapCapFactor *
                     here->MOS3w;
             GateBulkOverlapCap = model->MOS3gateBulkOverlapCapFactor *
                     EffectiveLength;
     ...
     ...

   And the new one:

     ...
     ...
         double EffectiveWidth;
     ...
     ...
              EffectiveWidth  = here->MOS3w - 2*model->MOS3widthNarrow
                                + model->MOS3widthAdjust;
              EffectiveLength = here->MOS3l - 2*model->MOS3latDiff
                                + model->MOS3lengthAdjust;
              GateSourceOverlapCap = model->MOS3gateSourceOverlapCapFactor *
                      here->MOS3m * EffectiveWidth;
              GateDrainOverlapCap = model->MOS3gateDrainOverlapCapFactor *
                      here->MOS3m * EffectiveWidth;
              GateBulkOverlapCap = model->MOS3gateBulkOverlapCapFactor *
                      here->MOS3m * EffectiveLength;
     ...
     ...

   A brief look at the new code shows that a new variable
`EffectiveWidth' appears and its value depends on the newly introduced
parameters `wd' and `xw', through `MOS3widthNarrow' and
`MOS3widthAdjust', respectively.  The values of `EffectiveLength' is
trimmed with the value of `xl' through `MOS3lengthAdjust'. The overlap
capacitances are multiplied by `EffectiveWidth' instead of `MOS3w'. The
`MOS3m' value has been discussed above.

   The `MOS3pzLoad()' function is very similar to `MOS3acLoad()' and
the code affected is almost identical to the one above.

   The `MOS3load()' function describes the model for large signals
analyses. The old code is:

     ...
     ...
      EffectiveLength = here->MOS3l - 2*model->MOS3latDiff;
         if( (here->MOS3tSatCurDens == 0)
             || (here->MOS3drainArea == 0)
             || (here->MOS3sourceArea == 0)) {
               DrainSatCur = here->MOS3tSatCur;
               SourceSatCur = here->MOS3tSatCur;
         } else {
               DrainSatCur  = here->MOS3tSatCurDens *
                              here->MOS3drainArea;
               SourceSatCur = here->MOS3tSatCurDens *
                              here->MOS3sourceArea;
         }
         GateSourceOverlapCap = model->MOS3gateSourceOverlapCapFactor
                                * here->MOS3w;
         GateDrainOverlapCap  = model->MOS3gateDrainOverlapCapFactor
                                * here->MOS3w;
         GateBulkOverlapCap   = model->MOS3gateBulkOverlapCapFactor
                                * EffectiveLength;
         Beta = here->MOS3tTransconductance * here->MOS3w/EffectiveLength;
         OxideCap = model->MOS3oxideCapFactor * EffectiveLength
                    * here->MOS3w;
     ...
     ...
            /*
             *.....body effect
             */
            gammas = model->MOS3gamma*fshort;
            fbodys = 0.5*gammas/(sqphbs+sqphbs);
            fbody = fbodys+model->MOS3narrowFactor/here->MOS3w;
            onfbdy = 1.0/(1.0+fbody);
            dfbdvb = -fbodys*dsqdvb/sqphbs+fbodys*dfsdvb/fshort;
            qbonco =gammas*sqphbs+model->MOS3narrowFactor*phibs/here->MOS3w;
            dqbdvb = gammas*dsqdvb+model->MOS3gamma*dfsdvb*sqphbs-
                     model->MOS3narrowFactor/here->MOS3w;
     ...
     ...
            /*
             *.....joint weak inversion and strong inversion
             */
            von = vth;
            if ( model->MOS3fastSurfaceStateDensity != 0.0 ) {
                csonco = CHARGE*model->MOS3fastSurfaceStateDensity
                         * 1e4 /*(cm**2/m**2)*/
                         * EffectiveLength*here->MOS3w/OxideCap;

     ...
     ...

   And the new code is:

     ...
     ...
      double EffectiveWidth;
     ...
     ...
      EffectiveWidth  = here->MOS3w - 2*model->MOS3widthNarrow
                        + model->MOS3widthAdjust;
      EffectiveLength = here->MOS3l - 2*model->MOS3latDiff
                        + model->MOS3lengthAdjust;
      if( (here->MOS3tSatCurDens == 0)
          || (here->MOS3drainArea == 0)
          || (here->MOS3sourceArea == 0)) {
            DrainSatCur = here->MOS3m * here->MOS3tSatCur;
            SourceSatCur = here->MOS3m * here->MOS3tSatCur;
       } else {
            DrainSatCur = here->MOS3m * here->MOS3tSatCurDens
                          * here->MOS3drainArea;
            SourceSatCur = here->MOS3m * here->MOS3tSatCurDens
                           * here->MOS3sourceArea;
       }
       GateSourceOverlapCap = model->MOS3gateSourceOverlapCapFactor
                              * here->MOS3m * EffectiveWidth;
       GateDrainOverlapCap  = model->MOS3gateDrainOverlapCapFactor
                              * here->MOS3m * EffectiveWidth;
       GateBulkOverlapCap   = model->MOS3gateBulkOverlapCapFactor
                              * here->MOS3m * EffectiveLength;
       Beta = here->MOS3tTransconductance
              * here->MOS3m * EffectiveWidth/EffectiveLength;
       OxideCap = model->MOS3oxideCapFactor * EffectiveLength
                  * here->MOS3m * EffectiveWidth;
     ...
     ...
            /*
             *.....body effect
             */
             gammas = model->MOS3gamma*fshort;
             fbodys = 0.5*gammas/(sqphbs+sqphbs);
             fbody  = fbodys+model->MOS3narrowFactor/EffectiveWidth;
             onfbdy = 1.0/(1.0+fbody);
             dfbdvb = -fbodys*dsqdvb/sqphbs+fbodys*dfsdvb/fshort;
             qbonco = gammas*sqphbs+model->MOS3narrowFactor
                       * phibs/EffectiveWidth;
             dqbdvb = gammas*dsqdvb+model->MOS3gamma*dfsdvb*sqphbs
                      - model->MOS3narrowFactor/EffectiveWidth;
     ...
     ...
            /*
             *.....joint weak inversion and strong inversion
             */
             von = vth;
             if ( model->MOS3fastSurfaceStateDensity != 0.0 ) {

                 csonco = CHARGE * model->MOS3fastSurfaceStateDensity *
                         1e4 /*(cm**2/m**2)*/
                         * EffectiveLength*EffectiveWidth
                         *  here->MOS3m/OxideCap;
     ...
     ...

   The "trick" is to substitute the `MOS3w' with the effective width
taking into account device multiplicity. Another point where device
width matters is the noise routine:`MOS3noise()'.  The oginal code
computes noise densities as follows:

     ...
     ...
     noizDens[MOS3FLNOIZ] *= model->MOS3fNcoef *
     				 exp(model->MOS3fNexp *
     				 log(MAX(FABS(inst->MOS3cd),N_MINLOG))) /
     				 (data->freq * inst->MOS3w *
     				 (inst->MOS3l - 2*model->MOS3latDiff) *
     				 model->MOS3oxideCapFactor * model->MOS3oxideCapFactor);
     ...
     ...

   The new code adds width narrowing and and multiplicity:

     ...
     ...
     noizDens[MOS3FLNOIZ] *= model->MOS3fNcoef *
     				 exp(model->MOS3fNexp *
     				 log(MAX(FABS(inst->MOS3cd),N_MINLOG))) /
     				 (data->freq *
     				 (inst->MOS3w - 2*model->MOS3widthNarrow) *
                                      inst->MOS3m *
     				 (inst->MOS3l - 2*model->MOS3latDiff) *
     				 model->MOS3oxideCapFactor * model->MOS3oxideCapFactor);
     ...
     ...

   Another  place in the code that needs changes is the device setup
routine `MOS3setup()'. The followig code adds support for the new
parameters:

     ...
     ...
             if(!model->MOS3lengthAdjustGiven) {
                 model->MOS3lengthAdjust = 0;
             }
             if(!model->MOS3widthNarrowGiven) {
                 model->MOS3widthNarrow = 0;
             }
             if(!model->MOS3widthAdjustGiven) {
                 model->MOS3widthAdjust = 0;
             }
     ...
     ...

   This code sets up the default values when the parameters are not
supplied by the user (since they are optional).

   Another function modified to support the new parameters is the
`MOS3temp()'. The old code is:

                 if(here->MOS3l - 2 * model->MOS3latDiff <=0) {
                     (*(SPfrontEnd->IFerror))(ERR_FATAL,
                             "%s: effective channel length less than zero",
                             &(here->MOS3name));
                     return(E_BADPARM);
                 }

   And the new one:

     ...
     ...
                 if(here->MOS3l - 2 * model->MOS3latDiff +
                                      model->MOS3lengthAdjust <1e-6) {
                     (*(SPfrontEnd->IFerror))(ERR_FATAL,
                             "%s: effective channel length less than zero",
                             &(here->MOS3name));
                     return(E_PARMVAL);
                 }


                 if(here->MOS3w - 2 * model->MOS3widthNarrow +
                                      model->MOS3widthAdjust <1e-6) {
                     (*(SPfrontEnd->IFerror))(ERR_FATAL,
                             "%s: effective channel width less than zero",
                             &(here->MOS3name));
                     return(E_PARMVAL);
                 }
     ...
     ...

   The changes add a check over device width that was not present in the
original code and rise an error if the result is less than one
micrometer, while the old code checked against zero.

   The last (but not least) function that needed some care is the
sensitivity load routine: `MOS3sLoad()'. The original code was:

     ...
     ...

                     EffectiveLength = here->MOS3l
                         - 2*model->MOS3latDiff;
                     if(EffectiveLength == 0) {
                         DqgsDp = 0;
                         DqgdDp = 0;
                         DqgbDp = 0;
                     }
                     else {
                         DqgsDp = model->MOS3type * qgs0 / EffectiveLength;
                         DqgdDp = model->MOS3type * qgd0 / EffectiveLength;
                         DqgbDp = model->MOS3type * qgb0 / EffectiveLength;
                     }
                 }
                 else {
                     DqgsDp = model->MOS3type * qgs0 / here->MOS3w;
                     DqgdDp = model->MOS3type * qgd0 / here->MOS3w;
                     DqgbDp = model->MOS3type * qgb0 / here->MOS3w;
                 }
     ...
     ...

   And the modified code is:

     ...
     ...
         double EffectiveWidth;
     ...
     ...
                     EffectiveLength = here->MOS3l
                         - 2*model->MOS3latDiff + model->MOS3lengthAdjust;
                     if(EffectiveLength == 0) {
                         DqgsDp = 0;
                         DqgdDp = 0;
                         DqgbDp = 0;
                     }
                     else {
                         DqgsDp = model->MOS3type * qgs0 / EffectiveLength;
                         DqgdDp = model->MOS3type * qgd0 / EffectiveLength;
                         DqgbDp = model->MOS3type * qgb0 / EffectiveLength;
                     }
                 }
                 else {
                     EffectiveWidth = here->MOS3w
                         - 2*model->MOS3widthNarrow + model->MOS3widthAdjust;
                     DqgsDp = model->MOS3type * qgs0 / EffectiveWidth;
                     DqgdDp = model->MOS3type * qgd0 / EffectiveWidth;
                     DqgbDp = model->MOS3type * qgb0 / EffectiveWidth;
                 }
     ...
     ...

   There was an error in the original implementation that did not take
into account lateral diffusion `MOS3LatDiff'. The other changes take
into account the effective (against drawn) device width.

   That's all folks! The changes needed to support the new parameters
are (shortly and badly) described. This section on MOS3 continues with
other fixes.

   MOS3 device reported only half of the Meyer capacitance without
adding the overlap capacitance contribution, when reporting to the
`.OP' printout or in the rawfile. The routine `MOS3ask()' was
responsible for this:

     ...
     ...
        case MOS3_CGS:
                 value->rValue = *(ckt->CKTstate0 + here->MOS3capgs);
                 return(OK);
             case MOS3_CGD:
                 value->rValue = *(ckt->CKTstate0 + here->MOS3capgd);
                 return(OK);
     ...
     ...
     case MOS3_CAPGS:
                 value->rValue = *(ckt->CKTstate0 + here->MOS3capgs);
                 return(OK);
     ...
     ...
             case MOS3_CAPGD:
                 value->rValue = *(ckt->CKTstate0 + here->MOS3capgd);
                 return(OK);
     ...
     ...
             case MOS3_CAPGB:
                 value->rValue = *(ckt->CKTstate0 + here->MOS3capgb);
                 return(OK);
     ...
     ...

   The new code is:

     ...
     ...
       case MOS3_CGS:
           value->rValue = 2* *(ckt->CKTstate0 + here->MOS3capgs);
           return(OK);
       case MOS3_CGD:
           value->rValue = 2* *(ckt->CKTstate0 + here->MOS3capgd);
           return(OK);
     ...
     ...
       case MOS3_CAPGS:
           value->rValue = 2* *(ckt->CKTstate0 + here->MOS3capgs);
     /* add overlap capacitance */
           value->rValue +=
                        (here->MOS3modPtr->MOS3gateSourceOverlapCapFactor)
                         * here->MOS3m
                         * (here->MOS3w
                            +here->MOS3modPtr->MOS3widthAdjust
                            -2*(here->MOS3modPtr->MOS3widthNarrow));
           return(OK);
     ...
     ...
       case MOS3_CAPGD:
           value->rValue = 2* *(ckt->CKTstate0 + here->MOS3capgd);
     /* add overlap capacitance */
           value->rValue +=
                        (here->MOS3modPtr->MOS3gateDrainOverlapCapFactor)
                         * here->MOS3m
                         * (here->MOS3w
                            +here->MOS3modPtr->MOS3widthAdjust
                            -2*(here->MOS3modPtr->MOS3widthNarrow));
           return(OK);
     ...
     ...
       case MOS3_CAPGB:
           value->rValue = 2* *(ckt->CKTstate0 + here->MOS3capgb);
     /* add overlap capacitance */
           value->rValue +=
                        (here->MOS3modPtr->MOS3gateBulkOverlapCapFactor)
                         * here->MOS3m
                         * (here->MOS3l
                            +here->MOS3modPtr->MOS3lengthAdjust
                            -2*(here->MOS3modPtr->MOS3latDiff));
           return(OK);
     ...
     ...

   The "Gmin" implementation across the substrate diodes of MOS3 was
incorrect, correcting this dramatically improved DC convergence. The
original code in `MOS3load()' was:

                 /*
                  * bulk-source and bulk-drain diodes
                  *   here we just evaluate the ideal diode current and the
                  *   corresponding derivative (conductance).
                  */


     next1:    if(vbs <= 0) {
                   here->MOS3gbs = SourceSatCur/vt;
                   here->MOS3cbs = here->MOS3gbs*vbs;
                   here->MOS3gbs += ckt->CKTgmin;
               } else {
                   evbs = exp(MIN(MAX_EXP_ARG,vbs/vt));
                   here->MOS3gbs = SourceSatCur*evbs/vt + ckt->CKTgmin;
                   here->MOS3cbs = SourceSatCur * (evbs-1);
               }
               if(vbd <= 0) {
                   here->MOS3gbd = DrainSatCur/vt;
                   here->MOS3cbd = here->MOS3gbd *vbd;
                   here->MOS3gbd += ckt->CKTgmin;
               } else {
                   evbd = exp(MIN(MAX_EXP_ARG,vbd/vt));
                   here->MOS3gbd = DrainSatCur*evbd/vt +ckt->CKTgmin;
                   here->MOS3cbd = DrainSatCur *(evbd-1);
               }

   The new corrected code is:

               /*
                *   bulk-source and bulk-drain diodes
                *   here we just evaluate the ideal diode current and the
                *   corresponding derivative (conductance).
                */

     next1:    if(vbs <= -3*vt) {
                   here->MOS3gbs = ckt->CKTgmin;
                   here->MOS3cbs = here->MOS3gbs*vbs-SourceSatCur;
               } else {
                   evbs = exp(MIN(MAX_EXP_ARG,vbs/vt));
                   here->MOS3gbs = SourceSatCur*evbs/vt + ckt->CKTgmin;
                   here->MOS3cbs = SourceSatCur*(evbs-1) + ckt->CKTgmin*vbs;
               }
               if(vbd <= -3*vt) {
                   here->MOS3gbd = ckt->CKTgmin;
                   here->MOS3cbd = here->MOS3gbd*vbd-DrainSatCur;
               } else {
                   evbd = exp(MIN(MAX_EXP_ARG,vbd/vt));
                   here->MOS3gbd = DrainSatCur*evbd/vt + ckt->CKTgmin;
                   here->MOS3cbd = DrainSatCur*(evbd-1) + ckt->CKTgmin*vbd;
               }

   In the "load current vector" section of the `MOS3load()' routine,
"Gmin" appeared in the calculation of `ceqbd' and `ceqbs':

         /*
          *  load current vector
          */
           ceqbs = model->MOS3type *
                   (here->MOS3cbs-(here->MOS3gbs-ckt->CKTgmin)*vbs);
           ceqbd = model->MOS3type *
                   (here->MOS3cbd-(here->MOS3gbd-ckt->CKTgmin)*vbd);

   The new code is:

         /*
          *  load current vector
          */
           ceqbs = model->MOS3type *
                   (here->MOS3cbs-(here->MOS3gbs)*vbs);
           ceqbd = model->MOS3type *
                   (here->MOS3cbd-(here->MOS3gbd)*vbd);

   The gm, gmb and gs calculations in them MOS3 model (in `MOD3load()'
were all wrong:

     ...
     ...
      /*
       *.....normalized drain current
       */
       cdnorm = cdo*vdsx;
       here->MOS3gm = vdsx;
       here->MOS3gds = vgsx-vth-(1.0+fbody+dvtdvd)*vdsx;
       here->MOS3gmbs = dcodvb*vdsx;
       /*
        *.....drain current without velocity saturation effect
        */
        cd1 = Beta*cdnorm;
        Beta = Beta*fgate;
        cdrain = Beta*cdnorm;
        here->MOS3gm = Beta*here->MOS3gm+dfgdvg*cd1;
        here->MOS3gds = Beta*here->MOS3gds+dfgdvd*cd1;
        here->MOS3gmbs = Beta*here->MOS3gmbs;
     ...
     ...
        cdrain = cdrain*xlfact;
        diddl = cdrain/(EffectiveLength-delxl);
        here->MOS3gm = here->MOS3gm*xlfact+diddl*ddldvg;
        gds0 = here->MOS3gds*xlfact+diddl*ddldvd;
        here->MOS3gmbs = here->MOS3gmbs*xlfact+diddl*ddldvb;
        here->MOS3gm = here->MOS3gm+gds0*dvsdvg;
        here->MOS3gmbs = here->MOS3gmbs+gds0*dvsdvb;
        here->MOS3gds = gds0*dvsdvd+diddl*dldvd;
     ...
     ...

   The code has been corrected as follows leading to much improved
convergence:

     ...
     ...
      /*
       *.....normalized drain current
       */
       cdnorm = cdo*vdsx;
       here->MOS3gm = vdsx;
       if ((here->MOS3mode*vds) > vdsat) here->MOS3gds = -dvtdvd*vdsx;
       else here->MOS3gds = vgsx-vth-(1.0+fbody+dvtdvd)*vdsx;
       here->MOS3gmbs = dcodvb*vdsx;
       /*
        *.....drain current without velocity saturation effect
        */
       cd1 = Beta*cdnorm;
       Beta = Beta*fgate;
       cdrain = Beta*cdnorm;
       here->MOS3gm = Beta*here->MOS3gm+dfgdvg*cd1;
       here->MOS3gds = Beta*here->MOS3gds+dfgdvd*cd1;
       here->MOS3gmbs = Beta*here->MOS3gmbs+dfgdvb*cd1;
     ...
     ...
       cd1 = cdrain;
       cdrain = cdrain*xlfact;
       diddl = cdrain/(EffectiveLength-delxl);
       here->MOS3gm = here->MOS3gm*xlfact+diddl*ddldvg;
       here->MOS3gmbs = here->MOS3gmbs*xlfact+diddl*ddldvb;
       gds0 = diddl*ddldvd;
       here->MOS3gm = here->MOS3gm+gds0*dvsdvg;
       here->MOS3gmbs = here->MOS3gmbs+gds0*dvsdvb;
       here->MOS3gds = here->MOS3gds*xlfact+diddl*dldvd+gds0*dvsdvd;

     /*
       here->MOS3gds = (here->MOS3gds*xlfact)+gds0*dvsdvd-
       (cd1*ddldvd/(EffectiveLength*(1-2*dlonxl+dlonxl*dlonxl)));
      */
     ...
     ...

   The Spice3 "fix" for the MOS3 gds discontinuity between the linear
and saturated regions works only if VMAX parameter is set to a non-zero
value. A tweak has been added for the zero case. The Spice3 code (in
`MOS3load()') was:

     ...
     ...
         /*
          *.....velocity saturation factor
          */
                 if ( model->MOS3maxDriftVel != 0.0 ) {
                     fdrain = 1.0/(1.0+vdsx*onvdsc);
                     fd2 = fdrain*fdrain;
                     arga = fd2*vdsx*onvdsc*onfg;
                     dfddvg = -dfgdvg*arga;
                     dfddvd = -dfgdvd*arga-fd2*onvdsc;
                     dfddvb = -dfgdvb*arga;
     ...
     ...

   The code in NGSPICE is:

     ...
     ...
         /*
          *.....velocity saturation factor
          */
                 if ( model->MOS3maxDriftVel > 0.0 ) {
                     fdrain = 1.0/(1.0+vdsx*onvdsc);
                     fd2 = fdrain*fdrain;
                     arga = fd2*vdsx*onvdsc*onfg;
                     dfddvg = -dfgdvg*arga;
                     if ((here->MOS3mode*vds) > vdsat) dfddvd = -dfgdvd*arga;
                     else dfddvd = -dfgdvd*arga-fd2*onvdsc;
                     dfddvb = -dfgdvb*arga;
     ...
     ...

   The critical voltages in `MOS3Temp()' were calculated without using
temperature corrected saturation current:

     ...
     ...
                       vt*log(vt/(CONSTroot2*model->MOS3jctSatCur));
           } else {
               here->MOS3drainVcrit =
                       vt * log( vt / (CONSTroot2 *
                       model->MOS3jctSatCurDensity * here->MOS3drainArea));
               here->MOS3sourceVcrit =
                       vt * log( vt / (CONSTroot2 *
                       model->MOS3jctSatCurDensity * here->MOS3sourceArea));
           }
     ...
     ...

   This have been fixed as follows:

     ...
     ...
                      vt*log(vt/(CONSTroot2*here->MOS3m*here->MOS3tSatCur));
          } else {
              here->MOS3drainVcrit =
                      vt * log( vt / (CONSTroot2 *
                        here->MOS3m *
                        here->MOS3tSatCurDens * here->MOS3drainArea));
                here->MOS3sourceVcrit =
                        vt * log( vt / (CONSTroot2 *
                        here->MOS3m *
                        here->MOS3tSatCurDens * here->MOS3sourceArea));
          }
     ...
     ...

   In `MOS3temp()' some parameters were computed without taking into
account temperature corrected parameters:

     ...
     ...
      here->MOS3f3d = czbd * model->MOS3bulkJctBotGradingCoeff
                      * sarg/ arg / model->MOS3bulkJctPotential
                      + czbdsw * model->MOS3bulkJctSideGradingCoeff
                      * sargsw/ arg /model->MOS3bulkJctPotential;
      here->MOS3f4d = czbd*model->MOS3bulkJctPotential*(1-arg*sarg)/
                      (1-model->MOS3bulkJctBotGradingCoeff)
                      + czbdsw*model->MOS3bulkJctPotential*(1-arg*sargsw)/
                      (1-model->MOS3bulkJctSideGradingCoeff)
                      -here->MOS3f3d/2*
                      (here->MOS3tDepCap*here->MOS3tDepCap)
                      -here->MOS3tDepCap * here->MOS3f2d;
      if(model->MOS3capBSGiven) {
              czbs=here->MOS3tCbs;
      } else {
             if(model->MOS3bulkCapFactorGiven) {
                     czbs=here->MOS3tCj*here->MOS3sourceArea;
             } else {
                     czbs=0;
             }
      }
     ...
     ...
      here->MOS3f3s = czbs * model->MOS3bulkJctBotGradingCoeff
                      * sarg/ arg / model->MOS3bulkJctPotential
                      + czbssw * model->MOS3bulkJctSideGradingCoeff
                      * sargsw/ arg / model->MOS3bulkJctPotential;
      here->MOS3f4s = czbs*model->MOS3bulkJctPotential*(1-arg*sarg)/
                             (1-model->MOS3bulkJctBotGradingCoeff)
                         + czbssw*model->MOS3bulkJctPotential*(1-arg*sargsw)/
                             (1-model->MOS3bulkJctSideGradingCoeff)
                         -here->MOS3f3s/2*
                             (here->MOS3tBulkPot*here->MOS3tBulkPot)
                         -here->MOS3tBulkPot * here->MOS3f2s;
             }
         }
     ...
     ...

   The corrected code is:

     ...
     ...
      here->MOS3f3d = czbd * model->MOS3bulkJctBotGradingCoeff
                      * sarg/ arg / here->MOS3tBulkPot
                      + czbdsw * model->MOS3bulkJctSideGradingCoeff
                      * sargsw/ arg / here->MOS3tBulkPot;
      here->MOS3f4d = czbd*here->MOS3tBulkPot*(1-arg*sarg)/
                      (1-model->MOS3bulkJctBotGradingCoeff)
                      + czbdsw*here->MOS3tBulkPot*(1-arg*sargsw)/
                      (1-model->MOS3bulkJctSideGradingCoeff)
                      -here->MOS3f3d/2*
                      (here->MOS3tDepCap*here->MOS3tDepCap)
                      -here->MOS3tDepCap * here->MOS3f2d;
      if(model->MOS3capBSGiven) {
              czbs = here->MOS3tCbs * here->MOS3m;
      } else {
             if(model->MOS3bulkCapFactorGiven) {
                     czbs=here->MOS3tCj*here->MOS3sourceArea * here->MOS3m;
             } else {
                    czbs=0;
             }
      }
     ...
     ...
      here->MOS3f3s = czbs * model->MOS3bulkJctBotGradingCoeff
                      * sarg/ arg / here->MOS3tBulkPot
                      + czbssw * model->MOS3bulkJctSideGradingCoeff
                      * sargsw/ arg /here->MOS3tBulkPot;
      here->MOS3f4s = czbs*here->MOS3tBulkPot*(1-arg*sarg)/
                      (1-model->MOS3bulkJctBotGradingCoeff)
                      + czbssw*here->MOS3tBulkPot*(1-arg*sargsw)/
                      (1-model->MOS3bulkJctSideGradingCoeff)
                      -here->MOS3f3s/2*
                      (here->MOS3tDepCap*here->MOS3tDepCap)
                      -here->MOS3tDepCap * here->MOS3f2s;
             }
         }

14.1.7 switch model
-------------------

14.1.8 current switch model
---------------------------

14.1.9 boh
----------

14.1.10 PN diode voltage limiting
---------------------------------

Spice3f voltage limiting across PN junctions did not perform limiting
on negative voltages, resulting in convergence problems. In NGSPICE
voltage limiting for PN diodes have been modified to work for negative
voltages too, improving convergence on calculations that rely on this
code.

ENHANCEMENT DATA:

Author:
     Alan Gillespie

File:
     `spicelib/devices/devsup.c'

Function:
     `DEVpnjlim()'

Affects:
     All devices model that uses that function: `BJT1-2', `BSIM3-4',
     `DIO', `EKV', `HFET2', `JFET1-2', `MES', `MESA', `MOS1-9'.

14.1.11 FET voltage limiting
----------------------------

In NGSPICE the calculation of VTSTLO is done according to the formula:
     vtstlo = fabs(vold - vto) + 1;
   While in spice3f the formula was:
     vtstlo = vtsthi/2 + 2;

ENHANCEMENT DATA:

Author:
     Alan Gillespie

File:
     `spicelib/devices/devsup.c'

Function:
     `DEVfetlim()'

Affects:
     All devices model that uses that function: `BSIM1-4',`HFET1-2',
     `JFET1-2', `MES', `MESA', `MOS1-9', `STAG', `EKV'.

14.1.12 Meyer model improvement
-------------------------------

The calculation of active gate capacitance in `devsup.c' has been
improved to achieve better convergence.

ENHACEMENT DATA:

Author:
     Alan Gillespie

File:
     `spicelib/devices/devsup.c'

Function:
     `DEVqmeyer()'

Affects:
     All devices model that uses that function: `MOS1-9'.

15 The BSIM3 Model Integration
******************************

BSIM3 compact model is a de-facto standard in the circuit simulation
world and is extensively supported in the NGSPICE simulator. The
original model dates back to the end of 1995. After almost ten years,
three major revisions have been released by the Berkeley Device Group.
NGSPICE supports all BSIM3 model revisions.

   We dedicated an entire chapter to the BSIM3 model since the procedure
followed to integrate it into NGSPICE equally applies to other models
from Berkeley's Device Group like BSIM4 and BSIMSOI. Most of the content
of this chapter is devoted to the latest release of BSIM3 available at
the time of writing: version 3.2 and its minor revisions 3.2.2, 3.2.3
and 3.2.4.  It is trivial to apply the same concepts to the older ones
(3.0 and 3.1).

   The BSIM3 integration into NGSPICE is the result of the merging of
three different sources: the original Berkeley's code and two enhanced
version, one supplied by Alan Gillespie and the other by Serban
Popescu. Both Alan and Serban enhanced the basic model adding
multiplicity support, though using two different approaches. Serban
added another enhancement, the "hdif" parameter.

   NGSPICE provides Berkeley's, Alan's and Serban's models, using
Alan's approach fot multiplicity support in Berkeley's code.

15.1 BSIM3 Revisions
====================

As previously said, due to the importance of BSIM3, NGSPICE includes all
its revisions. We have decide to assign different levels only to major
revisions and use the "version" model parameter to switch among minors.
The only exceptions to this rule are Serban's and Alan's model, they are
a special kind of BSIM3 version 3.1 and they are kept separate from the
Berkeley's model.

   NGSPICE has five different levels for BSIM3:

Major Revision         Minor Revisions        Level   Notes
BSIM3v3.2              3.2, 3.2.2, 3.2.3,     8       The latest release
                       3.2.4                          
BSIM3v1S               3.1                    49      Serban's code
BSIM3v1                3.1                    50      Berkeley's code
BSIM3v1A               3.1                    51      Alan's code
BSIM3v0                3.0                    52      Berkeley's code

   As you may see from the table above, level 8, the one officially
assigned by Berkeley Device Group,is reserved to the most recent major
revision of the code. All BSIM3 models support the "m" parameter
(multiplicity) but only Serban's one has the support for "hdif".

15.2 The integration process
============================

This section briefly describes how we integrated the BSIM3 model into
NGSPICE. The integration process of BSIM3 model started with the
download of the original code from Berkeley web site (device group). We
devoted much of the work on release 3.2 and backported changes to the
older ones. Our work on the BSIM model can be summarized in the
following points:

   * Restructuring code for spice3f interface.

   * Adding minor releases switches (where necessary).

   * Adding support for parallel simulation (CIDER).

   * Adding support for "m" parameter.

   * Restructuring code for NGSPICE integration.

   The first item is a necessary step for older models, since the device
interface changed between spice3e (the original interface for BSIM3
model) and spice3f and NGSPICE device interface is based on spice3f.
Changes consists is a shift in the position of `BSIM3states' in
`bsim3def.h' and in the addition of the `BSIM3unsetup()' function in
`b3set.c'.

   The next step is the inclusion of runtime switches to select code
for the different minor revisions that a release can have (well, this
is necessary only for release 3.2).

   The result of the two steps is a multirevision BSIM3 model with a
spice3f4/5 interface. Now we are ready to make the necessary
enhancements and the changes for integrating the model into NGSPICE.

   The third and fourth items in the list are the model enhancements:
the "parallel simulation support" is a feature inherited from the CIDER
simulator (built on top of NGSPICE) that allow the simulator to use
multiple processor elements to evaluate device code (making the
simulation faster). The parallel simulation is not yet enabled in
NGSPICE, but it will probably in the future. The "parallelization" code
basically consists in a series of switches that skip device evaluation
code if local processor (machine) has not been assigned to that
particular device instance.

   Device "multiplicity" is a feature often found in commercial
simulators, used to simulate many identical devices connected in
parallel. This feature is important because reduces the number of nodes
and equations in a circuit and makes the netlist more readable.

   Now we are ready to restructure the code to make it compatible with
the NGSPICE device interface, which is an extended version of the
spice3f4/5 one.

15.3 The multirevision code
===========================

BSIM3 release 3.2 has three minor revisions: 3.2.2, 3.2.3 and 3.2.4.
Reserving a different level for each is not a good solution, it will be
a waste of space and memory. The four (including 3.2) revisions differs
for a few lines of code only, so the ideai is to merge the code and
isolate revision dependent parts with runtime switches (the `switch'
statement). The modifications needed are minimal, but some work is
needed to avoid slow comparison between strings.

   As written before, the magic of revision selection is done via the
"version" model parameter, which appears on the model card. In BSIM3
version 3.2 this parameter is a floating point value, since earlier
releases were 3.0 and 3.1 and was easy to code revision into a real
number. With the release of 3.2.2 it changed to a string, for obvious
reasons (3.2.2 is not a real number). Since the "version" parameter was
used only for model checking, that was not a problem. In the
multirevision model, comparisons based on it appears in the device
evaluation code, where speed is critical, so we added a parameter
`BSIM3intVersion', defined in `bsim3def.h' as follows:

     ...
     ...
      char   *BSIM3version;

         /* The following field is an integer coding
          * of BSIM3version.
          */
         int    BSIM3intVersion;
     #define BSIM3V324  324       /* BSIM3 V3.2.4 */
     #define BSIM3V323  323       /* BSIM3 V3.2.3 */
     #define BSIM3V322  322       /* BSIM3 V3.2.2 */
     #define BSIM3V32   32        /* BSIM3 V3.2   */
     #define BSIM3V3OLD 0         /* Old model    */
         double BSIM3tox;
     ...
     ...

   The `BSIM3intVersion' will be used as argument to the `switch'
statement, because integer comparison is faster than string's one. The
correct value of the parameter is assigned in `BSIM3setup()' by the
code below:

     ...
     ...
     	/* If the user does not provide the model revision,
     		 * we always choose the most recent.
     		 */
     		if (!model->BSIM3versionGiven)
     			model->BSIM3version = "3.2.4";

     		/* I have added below the code that translate model string
     		 * into an integer. This trick is meant to speed up the
     		 * revision testing instruction, since comparing integer
     		 * is faster than comparing strings.
     		 * Paolo Nenzi 2002
     		 */
     		if (!strcmp (model->BSIM3version, "3.2.4"))
     			model->BSIM3intVersion = BSIM3V324;
     		else if (!strcmp (model->BSIM3version, "3.2.3"))
     			model->BSIM3intVersion = BSIM3V323;
     		else if (!strcmp (model->BSIM3version, "3.2.2"))
     			model->BSIM3intVersion = BSIM3V322;
     		else if (!strcmp (model->BSIM3version, "3.2"))
     			model->BSIM3intVersion = BSIM3V32;
     		else
     			model->BSIM3intVersion = BSIM3V3OLD;
     		/* BSIM3V3OLD is a placeholder for pre 3.2 revision
     		 * This model should not be used for pre 3.2 models.
     		 */
     ...
     ...

   When we need to switch the code we use a `switch' statement like the
following:


      /* Added revision dependent code */
     		  switch (model->BSIM3intVersion)
     		    {
     		    case BSIM3V324:
     			/* BSIM3v3.2.4 specific code */
     		    break;

     			case BSIM3V323:
     			/* BSIM3v3.2.3 specific code */
     			break;

     		    case BSIM3V322:
     			/* BSIM3v3.2.2 specific code */
     			break;
     		    case BSIM3V32:
     			/* BSIM3v3.2 specific code */
     			break;

     		    default:
     		    /* Old code */
     		    }

   The differences between minor revision fall in two categories:
modification in the evaluation code and bug fixes. The idea followed in
the merging was to leave out of the revision dependent code what was a
mere bug fix.

15.4 Device Multiplicity
========================

Spice3 (and thus NGSPICE) uses an approach called MNA (Modified Nodal
Analysis) to solve electrical circuits. MNA represents an electrical
circuits using a matrix containing devices' conductances and constraint
equations (if you need to know more, get a good book on circuit
theory). This matrix is built by summing the contribution of each
instance (another name for "element") in the circuit. The contribution
of each instance to the circuit matrix is called a "matrix stamp",
which is itself a matrix containing non zero elements only at positions
occupied by the device. It is very important to understand that row and
column index of the stamp must be consistent with the overall circuit
matrix, the elements of the stamp have the same indexes they will have
in the circuit matrix. Note that all stamps are each other independent,
and this property can be exploited to add parallelization to the
simulator (this is not new, CIDER uses this method).

   All the code in the model (every spice3 model) is needed to build
the matrix stamp for that particular instance of the device and for the
analysis type requested.

   If we add many (let's say "m") device in parallel, "m" identical
stamp are added to the circuit matrix. When we write "identical" we
mean that the stamps contain identical values but at different
locations. Each device has "external" and "internal" nodes, the former
are connected to devices' terminals and the latter are internal to the
device. It should be clear that nodes corresponding to terminals must
have the same node number and the same indexes in the matrix, since
devices appear in parallel, while other must be different because those
nodes are private to each instance.

   If we want to simulate "m" identical devices in parallel with a
single instance, its stamp must have an impact to the overall circuit
matrix equal to the "superposition" of the single instances' "m"
stamps. The term "superposition" is used instead of "sum" since we are
interested in the external behaviour of the parallel, not in its
internals. The matrix stamp of the "multiple" device is a stamp of a
single device whose conductances are "adjusted" to represent the
parallel situation. Doing this we discard the internal complexity of the
single instance while leaving intact the influence of the parallel to
the circuit. Reducing the complexity affects simulation speed, which is
increased because there are less equations (not useful to our purposes)
to solve and imposes less stress to simulator algorithms, resulting in
less convergence problems.

   We may say that a "multiple" device is an external representation of
many identical device connected in parallel.

   There are basically two approaches to build the equivalent stamp,
both based on scaling the conductances of the model by the multiplicity
value (the number of device to connect in parallel). The first approach
(used in NGSPICE BSIM3) scales the conductances in the matrix stamp,
when it is loaded into the overall matrix, and the other one scales the
conductances in the entire model code. Both approaches have advantages
and drawbacks, let's examine some of them.

   The first approach, i.e. scaling the conductances at loading time, is
advantageous because the stamp "loading" code is easy to spot and
because the modification consists simply in multiplying each line by
the multiplicity factor "m". Another advantage is that this approach
does not require a full analysis of the device code to isolate the
variables (they may be currents, resistances, etc.,  not only
conductances) that need to be scaled. The most important drawback is
that the evaluation code does not know anything about "multiplicity"
and then all internal computations are made for the "single" device. To
correct this, without interfering with the evaluation code, you need to
correct the routine that exports internal values (it is the so called
DEVask, where DEV is a placeholder for device's name).

   The second approach, i.e. scaling the variables in the evaluation
code, does not have the drawback of the previous one but require a full
code analysis which, in turn, means more time to complete.

15.4.1 Adding the "m" parameter
-------------------------------

The multiplicity parameter is an instance parameter. The first step is
to modify the code adding space for it in the various structures. The
structure `BSIM3instance' in `bsim3def.h' needs an entry for the new
parameter, its "given" flag and a numerical ID for the entry in the
`BSIM3pTable':

     ...
     ...
         double BSIM3w;
         double BSIM3m;
         double BSIM3drainArea;
     ...
     ...
         unsigned BSIM3wGiven :1;
         unsigned BSIM3mGiven :1;
         unsigned BSIM3drainAreaGiven :1;
     ...
     ...
     #define BSIM3_L 2
     #define BSIM3_M 15
     #define BSIM3_AS 3
     ...
     ...

   The `BSIM3pTable' structure in `b3.c' needs an entry too:

     ...
     ...
     IOP( "w",   BSIM3_W,      IF_REAL   , "Width"),
     IOP( "m",   BSIM3_M,      IF_REAL   , "Parallel multiplier"),
     IOP( "ad",  BSIM3_AD,     IF_REAL   , "Drain area"),
     ...
     ...

   Once the entries are created, it is necessary to set up the
bureaucracy needed to set and query the new parameter. In the setup
routine `BSIM3setup()' the following code should be added:

                 if (!here->BSIM3mGiven)
                     here->BSIM3m = 1;

   This states that if multiplicity is not given in the netlist, it
must be defaulted to one. To set the "given" flag the following code
should be added to `BSIM3param()':

             case BSIM3_M:
                 here->BSIM3m = value->rValue;
                 here->BSIM3mGiven = TRUE;
                 break;

   The last modification nedeed by model bureaucracy must be done in
`BSIM3ask()'.

   The following code should be added:

             case BSIM3_M:
                 value->rValue = here->BSIM3m;
                 return(OK);

   Now the model is ready to set, query, default and use the new
parameter. As discussed before, this model use the "first" approach,
thus only matrix loading code is affected by the new parameter. In the
`BSIM3load' routine the "Load Current Vector" and "Load Y Matrix"
section should become:

     ...
     ...
        (*(ckt->CKTrhs + here->BSIM3gNode) -= m*ceqqg);
        (*(ckt->CKTrhs + here->BSIM3bNode) -= m*(ceqbs + ceqbd + ceqqb));
        (*(ckt->CKTrhs + here->BSIM3dNodePrime) +=m*(ceqbd - cdreq - ceqqd));
        (*(ckt->CKTrhs + here->BSIM3sNodePrime) += m*(cdreq + ceqbs + ceqqg
     	                                                 + ceqqb + ceqqd));
        if (here->BSIM3nqsMod)
        *(ckt->CKTrhs + here->BSIM3qNode) += m*(cqcheq - cqdef);

        /*
         *  load y matrix
         */

        T1 = qdef * here->BSIM3gtau;
        (*(here->BSIM3DdPtr) += m*here->BSIM3drainConductance);
        (*(here->BSIM3GgPtr) += m*(gcggb - ggtg));
     ...
     ...
        *(here->BSIM3QspPtr) += m*(ggts - gcqsb);
        *(here->BSIM3QbPtr) += m*(ggtb - gcqbb);
     ...
     ...

   The "load y matrix" is not completely shown, each line is multiplied
by "m". The same method has been applied to `BSIM3acLoad()' routine:

     ...
     ...
                   m = here->BSIM3m;

                   *(here->BSIM3GgPtr +1) += m * xcggb;
                   *(here->BSIM3BbPtr +1) -= M * (xcbgb + xcbdb + xcbsb);
     ...
     ...
                       *(here->BSIM3QspPtr) += m * xgts;
                       *(here->BSIM3QbPtr) += m * xgtb;
                   }
     ...
     ...

   The pole-zero analysis uses a load routine (`BSIM3pzLoad()') very
similar to the one used by the AC analysis:

     ...
     ...
                 m = here->BSIM3m;

     			*(here->BSIM3GgPtr) += m * (xcggb * s->real);
     			*(here->BSIM3GgPtr + 1) += m * (xcggb * s->imag);
     ...
     ...
                     *(here->BSIM3QbPtr) += m * xgtb;
     				*(here->BSIM3QspPtr) += m * xgts;
     			}
     ...
     ...

   The noise analysis needs special attention, since it does not
directly uses a matrix load  routine. In this case was necessary to
study the noise models used by BSIM3 and to scale the parameters
affected by multiplicity. The following parameters were multiplied by
the value of `BSIM3m': `BSIM3cd' (drain current), `BSIM3weff'
(effective width), `BSIM3drainConductance', `BSIM3sourceConductance',
`BSIM3gm' (transconductance), `BSIM3gds' (drain to source conductance),
`BSIM3gmbs' (body source transconductance), `BSIM3qinv' (charge in the
channel).

   In 3.2.4 BSIM3 revision, a bugfix introduced the `BSIM3rds' (drain
to source resistance) parameter. Since this is a resistance it has been
divided by the value of `BSIM3m'.

   Now that we dealt with analyses code, the last piece of code to
modify is the `BSIM3ask()' routine. Again we have to identify what
parameters need to be scaled and multiply them by the multiplicity. If
you look at the code you will clearly see the affected parameters.

15.5 BSIM3 TNOM patch
=====================

All BSIM3 models, when implemented into Spice3f (NGSPICE), shows a bug
that affects simulations when the modelcard contains the TNOM keyword.
If you run consecutive times a netlist without reloading the deck, you
will get different answers with each run. Mike Smith discovered that
the bug hides in the functions `BSIM3mparam()' and `BSIM3setup()'. The
solutions (as extracted from Mike's post to `comp.lsi.cad'):

     In b3mpar.c look for the following code:-

             case  BSIM3_MOD_TNOM :
                 mod->BSIM3tnom = value->rValue;
                 mod->BSIM3tnomGiven = TRUE;
                 break;

     Change the second line so the code reads:-

             case  BSIM3_MOD_TNOM :
                 mod->BSIM3tnom = value->rValue + 273.15;
                 mod->BSIM3tnomGiven = TRUE;
                 break;

     In b3set.c, look for the following code:-

             if (!model->BSIM3tnomGiven)
                 model->BSIM3tnom = ckt->CKTnomTemp;
     	  else
                 model->BSIM3tnom = model->BSIM3tnom + 273.15;

     Delete the second and third lines to read:-

             if (!model->BSIM3tnomGiven)
                 model->BSIM3tnom = ckt->CKTnomTemp;

15.6 References for BSIM3 model
===============================

BSIM3 model is developed by the UC Berkeley Device Group, which
maintains a web site at the URL: `http://www-device.eecs.berkeley.edu/'
for all the model they develop.

   * BSIM3 home page:
     `http://www-device.eecs.berkeley.edu/~bsim3/latenews.html'

   * BSIM3 introduction:
     `http://www-device.eecs.berkeley.edu/~bsim3/intro.html'

   * BSIM3 contact page:
     `http://www-device.eecs.berkeley.edu/~bsim3/contact.html'

16 EKV Model
************

da scrivere



Tag Table:
Node: Top1839
Node: Preface4882
Node: Acknowledgements6934
Node: Release Notes9189
Node: Introduction22342
Node: NGSPICE Compilation27400
Node: Extracting the archive27957
Node: Configuring NGSPICE28927
Node: Compiling NGSPICE35396
Node: Supported systems36235
Node: Platform specific issues38434
Node: Supported Analyses39539
Node: Types of Analysis39844
Node: DC Analysis40214
Node: AC Small-Signal Analysis41406
Node: Transient Analysis42287
Node: Pole-Zero Analysis42850
Node: Small-Signal Distortion Analysis44213
Node: Sensitivity Analysis45452
Node: Noise Analysis46374
Node: Analysis at Different Temperatures47448
Node: Convergence52829
Node: Circuit Description53975
Node: General Structure and Conventions54248
Node: Basics57572
Node: Title Line57850
Node: END58173
Node: Comments58436
Node: Device Models58928
Node: Subcircuits61036
Node: SUBCKT61684
Node: ENDS62777
Node: Subcircuit Calls63280
Node: INCLUDE63672
Node: Circuit Elements and Models64306
Node: General options and information65180
Node: Simulating more devices in parallel65520
Node: Technology scaling66685
Node: Model binning66927
Node: Elementary Devices67142
Node: Resistors67586
Node: Semiconductor Resistors69992
Node: Semiconductor Resistor Model (R)71289
Node: Capacitors74986
Node: Semiconductor Capacitors76678
Node: Semiconductor Capacitor Model (C)77758
Node: Inductors80592
Node: Inductor model82172
Node: Coupled (Mutual) Inductors84883
Node: Switches85447
Node: Switch Model (SW/CSW)86432
Node: Voltage and Current Sources88971
Node: Independent Sources89251
Node: Pulse92250
Node: Sinusoidal93305
Node: Exponential94223
Node: Piece-Wise Linear95532
Node: Single-Frequency FM96084
Node: Linear Dependent Sources96940
Node: Linear Voltage-Controlled Current Sources97656
Node: Linear Voltage-Controlled Voltage Sources98306
Node: Linear Current-Controlled Current Sources98868
Node: Linear Current-Controlled Voltage Sources99653
Node: Non-linear Dependent Sources100318
Node: Transmission Lines103729
Node: Lossless Transmission Lines104118
Node: Lossy Transmission Lines105890
Node: Lossy Transmission Line Model (LTRA)106549
Node: Uniform Distributed RC Lines (Lossy)112033
Node: Uniform Distributed RC Model (URC)112803
Node: Transistors and Diodes114816
Node: Junction Diodes116939
Node: Diode Model (D)118423
Node: Diode Equations123097
Node: Bipolar Junction Transistors (BJTs)129760
Node: BJT Models (NPN/PNP)131162
Node: Junction Field-Effect Transistors (JFETs)142628
Node: JFET Models (NJF/PJF)143721
Node: MOSFETs146224
Node: MOSFET Models (NMOS/PMOS)148439
Node: MESFETs165297
Node: MESFET Models (NMF/PMF)165574
Node: Analyses and Output Control168349
Node: Simulator Variables (.OPTIONS)169856
Node: Initial Conditions174875
Node: Specify Initial Node Voltage Guesses175139
Node: Set Initial Conditions175894
Node: Analyses177785
Node: AC Small-Signal AC Analysis178229
Node: DC Transfer Function179177
Node: DISTRO Distortion Analysis180394
Node: NOISE Noise Analysis186184
Node: OP Operating Point Analysis187483
Node: PZ Pole-Zero Analysis188177
Node: SENS; DC or Small-Signal AC Sensitivity Analysis189550
Node: TF Transfer Function Analysis190704
Node: TRAN Transient Analysis191575
Node: Batch Output193271
Node: SAVE193495
Node: PRINT194339
Node: PLOT196253
Node: FOUR Fourier Analysis of Transient Analysis Output197453
Node: Interactive Interpreter198338
Node: Expressions202769
Node: Command Interpretation208969
Node: Commands210771
Node: AC211685
Node: Alias212050
Node: Alter212365
Node: Asciiplot213206
Node: Aspice213948
Node: Bug214398
Node: Cd214857
Node: Destroy215136
Node: DC215397
Node: Define215748
Node: Delete216626
Node: Diff217039
Node: Display217560
Node: Echo218407
Node: Edit218620
Node: Fourier219088
Node: Hardcopy219950
Node: Help220381
Node: History220862
Node: Iplot221251
Node: Jobs221612
Node: Let222031
Node: Linearize222567
Node: Listing223409
Node: Load224153
Node: Op224506
Node: Plot224804
Node: Print226859
Node: Quit227680
Node: Rehash227897
Node: Reset228317
Node: Reshape228851
Node: Resume229617
Node: Rspice229904
Node: Run231044
Node: Rusage231651
Node: Save233141
Node: Sens234390
Node: Set235072
Node: Setcirc235795
Node: Setplot236193
Node: Settype237068
Node: Shell237396
Node: Shift237724
Node: Show238130
Node: Showmod239534
Node: Source240048
Node: Status241093
Node: Step241370
Node: Stop241637
Node: Tf243421
Node: Trace243910
Node: Tran244282
Node: Transpose244618
Node: Unalias245678
Node: Undefine245929
Node: Unset246204
Node: Version246455
Node: Where248561
Node: Write249457
Node: Xgraph250263
Node: While - End250903
Node: Repeat - End251218
Node: Dowhile - End251530
Node: Foreach - End251865
Node: If - Then - Else252288
Node: Label252744
Node: Goto253019
Node: Continue253415
Node: Break253750
Node: Variables254298
Node: Bugs268421
Node: Bibliography270788
Node: Example Circuits273174
Node: Differential Pair273463
Node: MOSFET Characterization274191
Node: RTL Inverter274813
Node: Four-Bit Binary Adder275534
Node: Transmission-Line Inverter278089
Node: Model and Device Parameters278903
Node: Uniform RC line281997
Node: Arbitrary Source284081
Node: Bipolar Junction Transistor285223
Node: BSIM1 Berkeley Short Channel IGFET Model295547
Node: BSIM2 Berkeley Short Channel IGFET Model305731
Node: Fixed capacitor321060
Node: Current controlled current source323115
Node: Linear current controlled current source324388
Node: Current controlled ideal switch325691
Node: Junction Diode model328248
Node: Inductor332089
Node: Mutual inductors333425
Node: Independent current source334161
Node: Junction Field effect transistor336794
Node: Lossy transmission line342100
Node: GaAs MESFET model346239
Node: Level 1 MOSfet model351663
Node: Level 2 MOSfet model362168
Node: Level 3 MOSfet model373181
Node: Level 6 MOSfet model384538
Node: Simple linear resistor395357
Node: Ideal voltage controlled switch397545
Node: Lossless transmission line400157
Node: Voltage controlled current source402502
Node: Voltage controlled voltage source404252
Node: Independent voltage source405991

End Tag Table
