     [file version.texi not included]

     INFO-DIR-SECTION Simulation
     START-INFO-DIR-ENTRY
     * Ngspice: (ngspice).            General-purpose circuit simulation program for
                                      nonlinear dc, nonlinear transient, and linear
                                      ac analyses
     END-INFO-DIR-ENTRY

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

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

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.

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
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 , Warden of the Kings Ale

Acknowledgements
****************

     [file AUTHORS not included]

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.

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

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

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.

NGSPICE Compilation
*******************

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.

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).

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.

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/.

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 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 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 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.

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.

Supported Analyses
******************

This chapter introduces the analyses available in NGSPICE.

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

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.

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.

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.

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.

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.

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).

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.

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.

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.

Circuit Description
*******************

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).

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

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.

.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.

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.

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.

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.

.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.

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.

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.

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.

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).

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

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.

Technology scaling
------------------

Still to be implemented and written.

Model binning
-------------

Still to be implemented and written.

Elementary Devices
==================

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.

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 (see 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.

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

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

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 (see 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 (see Capacitors).

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.

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

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 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
NT        number of turns
-                   0.0    10
MU        relative magnetic permeability
H/meters            0.0    -

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.

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.

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.

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.

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

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)).

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.

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 factor)   0.0   1/seconds

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))

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  |

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.

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    |                            |

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.

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).

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.

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.

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).

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.

Transmission Lines
==================

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.

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.

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 unit   1   0.5
ABS   breakpoint control   1   5
NOSTEPLIMIT   don't limit timestep to less than line delay
flag   not set   set
NOCONTROL   don't do complex timestep control
flag   not set   set
LININTERP   use linear interpolation
flag   not set   set
MIXEDINTERP   use linear when quadratic seems bad
not set   set
COMPACTREL   special reltol for history compaction
flag   RELTOL   1.0e-3
COMPACTABS   special abstol for history compaction
ABSTOL   1.0e-9
TRUNCNR   use Newton-Raphson method for timestep control
flag   not set   set
TRUNCDONTCUT   don't limit timestep to keep impulse-response
errors low   flag   not set   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.

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).

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 length
A/m   0   -
RSPERL   Diode Resistance per unit length
Z/m   0   -

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.

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.

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 (IKF)    forward knee current   A   1.0e-3   1.0e-6
IK          reverse knee current   A   1.0e-3   1.0e-6
IS (JS)     saturation current     A   1.0e-14   1.0e-16   area
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 (CJ0)    zero-bias junction bottowall capacitance   F   0.0   2pF   area
CJP (CJSW)   zero-bias junction sidewall capacitance   F   0.0   .1pF   perim.
FC           coefficient for forward-bias depletion bottomwall capacitance formula
-   0.5   -
FCS          coefficient for forward-bias depletion sidewall capacitance formula
-   0.5   -
M (MJ)       Area junction grading coefficient   -   0.5   0.5
MJSW         Periphery junction grading coefficient   -   0.33   0.5
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 temperature   C   27   50
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

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)

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.

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
vertical geometry, -1 for
lateral geometry.
(level 2 only)                 1
1.0e-15
IS       transport saturation current   A   1.0e-16
1.0e-15   area
ISS      reverse saturation current,
substrate-to-collector for
vertical device or
substrate-to-base for lateral
(level 2 only)                      A   1.0e-16
1.0e-15   area

BF       ideal maximum forward beta     -   100   100
NF       forward current emission
coefficient                    -   1.0   1
VAF      forward Early voltage          V   infinite   200
IKF      corner for forward beta
current roll-off               A   infinite
0.01   area
ISE      B-E leakage saturation current   A   0   1.0e-13
area
NE       B-E leakage emission coefficient   -   1.5   2
BR       ideal maximum reverse beta   -   1   0.1
NR       reverse current emission coefficient   -   1
1
VAR      reverse Early voltage   V   infinite   200
IKR      corner for reverse beta high current roll-off
A   infinite   0.01   area
ISC      B-C leakage saturation current
(area is "areab" for vertical
devices and "areac" for lateral)   A   0
1.0e-13     area

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

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.

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 parameter (L)
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 (C_gs)
F   0   5pF   *
CGD   zero-bias G-D junction capacitance (C_gs)
F   0   1pF   *
PB   gate junction potential   V   1   0.6
IS   gate junction saturation current (I_S)
A   1.0e-14   1.0e-14   *
B   doping tail parameter   -   1   1.1
KF   flicker noise coefficient   -   0
AF   flicker noise exponent   -   1
FC   coefficient for forward-bias depletion capacitance formula
-   0.5
TNOM   parameter measurement temperature
^oC   27   50

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.

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_T0)
V   0.0   1.0
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 and MOS2 only) (L)
1/V   0.0   0.02
RD      drain ohmic resistance
Z   0.0   1.0
RS      source ohmic resistance
Z   0.0   1.0
CBD     zero-bias B-D junction capacitance
F   0.0   20fF
CBS     zero-bias B-S junction capacitance
F   0.0   20fF
IS      bulk junction saturation current (I_S)
A   1.0e-14   1.0e-15
PB      bulk junction potential
V   0.8   0.87
CGSO    gate-source overlap capacitance per meter channel width
F/m   0.0   4.0e-11
CGDO    gate-drain overlap capacitance per meter channel width
F/m   0.0   4.0e-11
CGBO    gate-bulk overlap capacitance per meter channel length
F/m   0.0   2.0e-10
RSH     drain and source diffusion sheet resistance
Z/[]   0.0   10.0
CJ      zero-bias bulk junction bottom cap. per sq-meter of junction area
F/m^2   0.0   2.0e-4
MJ      bulk junction bottom grading coeff.
-   0.5   0.5
CJSW    zero-bias bulk junction sidewall cap. per meter of junction perimeter
F/m   0.0   1.0e-9
MJSW    bulk junction sidewall grading coeff.
-   0.50(level1), 0.33(level2, 3)
JS      bulk junction saturation current per sq-meter of junction area
A/m^2   1.0e-8
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 opp. to substrate, -1 same as substrate, 0  Al gate
-   1.0
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 degradation (MOS2 only)
V/cm   1.0e4   1.0e4
UEXP    critical field exponent in mobility degradation (MOS2 only)
-   0.0   0.1
UTRA    transverse field coeff. (mobility) (deleted for MOS2)
-   0.0   0.3
VMAX    maximum drift velocity of carriers
m/s   0.0   5.0e4
NEFF    total channel-charge (fixed and mobile) coefficient (MOS2 only)
-   1.0   5.0
KF      flicker noise coefficient
-   0.0   1.0e-26
AF      flicker noise exponent
-   1.0   1.2
FC      coefficient for forward-bias depletion capacitance formula
-   0.5
DELTA   width effect on threshold voltage (MOS2 and MOS3)
-   0.0   1.0
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 only)
-   0.2   0.5
TNOM    parameter measurement temperature
^oC   27   50

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 degradation
coefficient                                              V^-1        *
U1       zero-bias velocity saturation coefficient                Mm/V          *
X2MZ     sens. of mobility to substrate bias at V_ds=0          cm^2/V-s      *
X2E      sens. of drain-induced barrier lowering effect to
substrate bias                                           V^-1        *
X3E      sens. of drain-induced barrier lowering effect to
drain bias at V_ds=V_dd                                  V^-1        *
X2U0     sens. of transverse field mobility degradation
effect to substrate bias                                 V^2        *
X2U1     sens. of velocity saturation effect to substrate
bias                                                    MmV^2       *
MUS      mobility at zero substrate bias and at V_ds=V_dd        cm^2/V^2-s
X2MS     sens. of mobility to substrate bias at V_ds=V_dd        cm^2/V^2-s     *
X3MS     sens. of mobility to drain bias at V_ds=V_dd            cm^2/V^2-s     *
X3U1     sens. of velocity saturation effect on drain bias
at V_ds=V_dd                                            MmV^2       *
TOX      gate oxide thickness                                    Mm
TEMP     temperature at which parameters were measured           C
VDD      measurement bias range                                  V
CGDO     gate-drain overlap capacitance per meter channel
width                                                   F/m
CGSO     gate-source overlap capacitance per meter channel
width                                                   F/m
CGBO     gate-bulk overlap capacitance per meter channel
length                                                  F/m
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 resistance              Z/[]
JS       source drain junction current density                    A/m^2
PB       built in potential of source drain junction              V
MJ       Grading coefficient of source drain junction             -
BSW      built in potential of source, drain junction
sidewall                                                 V
MJSW     grading coefficient of source drain junction
sidewall                                                 -
CJ       Source drain junction capacitance per unit area          F/m^2
CJSW     source drain junction sidewall capacitance per
unit length                                              F/m
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.

MESFETs
-------

General form:

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

Examples:

       Z1 7 2 3 ZM1 OFF

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
depletion capacitance formula         -              0.5

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.

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.

Initial Conditions
==================

.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.

.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.

Analyses
========

.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.

.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.

.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.

.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).

.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).

.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'.

.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).

.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.

.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.

Batch Output
============

.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.

.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.

.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.

.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).

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.

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.

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.

Commands
========

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.

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.

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 "]".

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.

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.

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.)

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.

Destroy: Delete a data set
--------------------------

General Form:

          destroy [plotnames | all]

Release the memory holding the data for the  specified runs.

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.

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

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).

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.

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).

Echo: Print text
----------------

General Form:

          echo [text...]

Echos the given text to the screen.

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.

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.

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.

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.

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.

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.

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.

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.

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.

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.

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.

Op*: Perform an operating point analysis
----------------------------------------

General Form:

          op

Do an operating point analysis.  See the previous sections of this manual for more details.

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.

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.

Quit: Leave Ngspice or Nutmeg
-----------------------------

General Form:

          quit

Quit nutmeg or ngspice.

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).

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.

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.

Resume*: Continue a simulation after a stop
-------------------------------------------

General Form:

          resume

Resume a simulation after a stop or interruption (control-C).

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.

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.

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".

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.

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).

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.

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.

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.

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.

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.

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.

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.

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".

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.

Status*: Display breakpoint information
---------------------------------------

General Form:

          status

Display all of the traces and breakpoints currently in effect.

Step*: Run a fixed number of timepoints
---------------------------------------

General Form:

          step [number]

Iterate number times, or once, and then stop.

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.

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 ->

     This command may not be available on your environment, if it is not available, please send analogous information when submitting bug reports.

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.

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.

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.

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]

Unalias: Retract an alias
-------------------------

General Form:

          unalias [word ...]

Removes any aliases present for the words.

Undefine: Retract a definition
------------------------------

General Form:

          undefine function

Definitions for the named user-defined functions are deleted.

Unset: Clear a variable
-----------------------

General Form:

          unset [word ...]

Clear the value of the specified variable(s) (word).

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.

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.

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.

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.

Control Structures
==================

While - End
-----------

General Form:

          while condition
            statement
            ...
          end

While condition, an arbitrary algebraic expression, is true, execute the statements.

Repeat - End
------------

General Form:

          repeat [number]
            statement
            ...
          end

Execute the statements number times, or forever if no argument is given.

Dowhile - End
-------------

General Form:

          dowhile condition
            statement
            ...
          end

The same as while, except that the condition is tested after the statements are executed.

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).

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.

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.

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).

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.

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.

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

INIT FILES
==========

Ngspice reads some initialization information and paths from a file called "spinit" or "tclspinit" (the latter if you have compiled tclspice). The init file is read by ngspice or ngnutmeg as they start. The init script contains spice commands (interactive commands). The following example show the standard ngspice init file.

     * Standard spice and nutmeg init file
     alias exit quit
     alias acct rusage all
     set x11lineararcs

     *unset brief

     strcmp __flag $program "ngspice"
     if $__flag = 0

     *set numparams

     * For SPICE2 POLYs, edit the below line to point to the location
     * of your codemode.
      codemodel /usr/local/lib/spice/spice2poly.cm

     * The other codemodels
      codemodel /usr/local/lib/spice/analog.cm
      codemodel /usr/local/lib/spice/digital.cm
      codemodel /usr/local/lib/spice/xtradev.cm
      codemodel /usr/local/lib/spice/xtraevt.cm

     end
     unset __flag

The spice init file location depends of the operating system you are running and the configuration parameters.

The init file is the best place to put commands you always input when the simulator starts.

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.

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.

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

Example Circuits
****************

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

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

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

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

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

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.

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             |
      ------------------------------------------------------------

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                           |
      ------------------------------------------------------------

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.                      |
      ------------------------------------------------------------

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                 |
      ------------------------------------------------------------------------

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     |
      ---------------------------------------------------------------

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                 |
      ------------------------------------------------------------

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                              |
      ------------------------------------------------------------

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                              |
      ------------------------------------------------------------

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                        |
      ------------------------------------------------------------

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                       |
      ------------------------------------------------------------

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
     |                                                            |
      -------------------------------------------------------------

mutual: Mutual inductors
========================

      ------------------------------------------------------------
     |        mutual - instance parameters (input-output)        |
     |-----------------------------------------------------------+
     | k                 Mutual inductance                       |
     | coefficient       (null)                                  |
     | inductor1         First coupled inductor                  |
     | inductor2         Second coupled inductor                 |
      ------------------------------------------------------------

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            |
      ------------------------------------------------------------

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                      |
      ------------------------------------------------------------

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  |
      ------------------------------------------------------------

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                        |
      ------------------------------------------------------------

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              |
      ------------------------------------------------------------

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              |
      ------------------------------------------------------------

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              |
      ------------------------------------------------------------

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              |
      ------------------------------------------------------------

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       |
      ------------------------------------------------------------

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                   |
      ------------------------------------------------------------

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            |
      ------------------------------------------------------------

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                                   |
      ------------------------------------------------------------

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                                   |
      ------------------------------------------------------------

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                     |
      ------------------------------------------------------------

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.

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)

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.

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.

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.

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);

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
                  */
     ...
     ...

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;
             }
         }

switch model
------------

current switch model
--------------------

boh
---

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.

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.

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.

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.

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, 3.2.4    8   The latest release
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".

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.

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.

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.

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.

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;

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

EKV Model
*********

da scrivere