spice.0

spice中支持多层次元件模型仿真的可单独运行的插件源码

20 March 1986                                            SPICE(1)



NAME
     spice - circuit simulator

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

DESCRIPTION
     This manual page describes the commands available for
     interactive use of SPICE3. For details of circuit descrip-
     tions and the process of simulating a circuit, see the
     SPICE3 User's Manual.  The commands available are a superset
     of those available for nutmeg - only the additional commands
     available in SPICE3 are described here.  You should be fami-
     liar with the manual page for nutmeg(1) before reading this
     manual page.

     Arguments are:

     -n (or -N)
          Don't try to source the file ".spiceinit" upon startup.
          Normally SPICE3 tries 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 _m_f_b name
          term.

     -b (or -B)
          Run in batch mode. SPICE3 will read the standard input
          or the specified input file and do the simulation. Note
          that if the standard input is not a terminal, SPICE3
          will default to batch mode, unless the -i flag is
          given.

     -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 spice daemon.

     -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.

     -r rawfile (or -R rawfile)
          Use rawfile as the default file into which the results
          of the simulation are saved.



                                                                1






SPICE(1)                                            20 March 1986



     Further arguments are taken to be SPICE3 input decks, which
     are read and saved. (If batch mode is requested then they
     are run immediately.)

     SPICE3 will accept any SPICE2 input decks, and output ascii
     plots, fourier analyses, and node printouts as specified in
     .plot, .four, and .print cards.  If a out parameter is given
     on a .width card, the effect is the same as set width = ....
     Since SPICE3 ascii plots do not use multiple ranges, how-
     ever, if vectors together on a .plot card have different
     ranges they will not provide as much information as they
     would in SPICE2. The output of SPICE3 is also much less ver-
     bose than SPICE2, in that the only data printed is that
     requested by the above cards.

     Vector names are the same as in nutmeg, with this addition:
     a name such as @name[param], where name is either the name
     of a device instance or model, denotes the value of the
     param parameter of the device or model. See the SPICE3
     User's Manual 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 vari-
     ables for convenience for command scripts.

     SPICE3 commands are as follows (these are only those com-
     mands not also available in nutmeg - consult the nutmeg
     manual page for more commands):

     setcirc [circuit name]
          Change the current circuit. The current circuit is the
          one that is used for the simulation commands below.
          When a circuit is loaded with the _s_o_u_r_c_e command (see
          below) it becomes the current circuit.

     op [.op card args]
          Do an operating point analysis.

     tran [.tran card args]
          Do a transient analysis.

     ac [.ac card args]
          Do an ac analysis.

     dc [.dc card args]
          Do a dc transfer curve analysis.

     listing [logical] [physical] [deck] [expand]
          Print a listing of the current circuit. 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



2






20 March 1986                                            SPICE(1)



          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 will be printed
          with all subcircuits expanded.

     edit [file]
          Print the current SPICE3 deck 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 origonal deck.
          If a filename is given, then edit that file and load
          it, making the circuit the current one.

     resume
          Resume a simulation after a stop.

     show Show a device parameter.

     alter
          Alter a device parameter.

     state
          Print the state of the circuit.  (This command is
          largely unimplemented.)

     save [all] [output ...]  or .save [all] [output ...]
          Save a set of outputs, discarding the rest. If a node
          has been mentioned in a save command, it will appear in
          the working plot after a run has completed, or in the
          rawfile if spice is run in batch mode. If a node is
          traced or plotted (see below) it will also be saved.
          For backward compatibility, if there are no save com-
          mands given, all outputs are saved.

     stop [ after n] [ when something cond something ] ...
          Set a breakpoint. The argument after n means stop after
          n iteration number n, and the argument when something
          cond something means stop when the first something is
          in the given relation with the second something, 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), and 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 any-
          way).  The somethings above may be node names in the
          running circuit, or real values.  If more than one con-
          dition is given, e.g.  stop after 4 when v(1) > 4 when
          v(2) < 2, the conjunction of the conditions is implied.

     trace [ node ...]
          Trace nodes. Every iteration the value of the node is



                                                                3






SPICE(1)                                            20 March 1986



          printed to the standard output.

     iplot [ node ...]
          Incrementally plot the values of the nodes while SPICE3
          runs.

     step [number]
          Iterate number times, or once, and then stop.

     status
          Display all of the traces and breakpoints currently in
          effect.

     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
          aren't printed.)

     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 deck. The circuit
          can then be re-run. (Note: this command used to be end
          in SPICE 3a5 and earlier versions -- end is now used
          for control structures.)  The run command will take
          care of this automatically, so this command should not
          be necessary...

     run [rawfile]
          Run the simulation as specified in the input file. If
          there were any of the control cards .ac, .op, .tran, or
          .dc, they are executed. The output is put in rawfile if
          it was given, in addition to being available interac-
          tively.

     source file
          Read the SPICE3 input file file. Nutmeg and SPICE3 com-
          mands may be included in the file, and must be enclosed
          between the lines _a_r_e _e_x_e_c_u_t_e_d _i_m_m_e_d_i_a_t_e_l_y _a_f_t_e_r _t_h_e
          _c_i_r_c_u_i_t _i_s _l_o_a_d_e_d, _s_o _a _c_o_n_t_r_o_l _l_i_n_e _o_f _a_c ... will
          work the same as the corresponding ._a_c 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 ._s_p_i_c_e_i_n_i_t.  Thus, a
          SPICE3 command script must begin with a blank line and
          then with a ._c_o_n_t_r_o_l line.  Also, any line beginning
          with the characters *# is considered a control line.
          This makes it possible to imbed commands in SPICE3
          input files that will be ignored by earlier versions of
          SPICE.  _N_o_t_e: in spice3a7 and before, the ._c_o_n_t_r_o_l and
          ._e_n_d_c lines were not needed, and any line beginning



4






20 March 1986                                            SPICE(1)



          with the name of a front-end command would be executed.

     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 will be interpolated onto a
          linear time scale, which is determined by the values of
          tstep, tstart, and tstop in the currently active tran-
          sient analysis.  The currently loaded deck 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 SPICE3 doesn't output
          the results from a transient analysis in the same
          manner that SPICE2 did.

     There are several set variables that SPICE3 uses but nutmeg
     does not. They are:

                     editor
                     The editor to use for the edit command.

                     modelcard
                     The name of the model card (normally
                     .model).

                     noaskquit
                     Do not check to make sure that there are no
                     circuits suspended and no plots unsaved.
                     Normally SPICE3 will warn the user when he
                     tries to quit if this is the case.

                     nobjthack
                     Assume that BJT's have 4 nodes.

                     noparse
                     Don't attempt to parse decks 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 a deck has
                     .include's.

                     subend
                     The card to end subcircuits (normally
                     .ends).

                     subinvoke



                                                                5






SPICE(1)                                            20 March 1986



                     The prefix to invoke subcircuits (normally
                     x).

                     substart
                     The card to begin subcircuits (normally
                     .subckt).

     There are a number of rusage parameters available, in addi-
     tion to the ones available in nutmeg:



     If there are subcircuits in the input file, SPICE3 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 sub-
     circuit 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 for-
     mal 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'.

VMS NOTES
     The standard suffix for rawspice files in VMS is ".raw".

     You may have to redefine the value EDITOR if you wish to use
     the edit command, since the default for VMS is "vi".

SEE ALSO
     nutmeg(1), sconvert(1), spice(1), mfb(3), writedata(3)
     SPICE3 User's Guide

AUTHORS
     SPICE3:  Tom Quarles ([e-mail])
     nutmeg / User interface: Wayne Christopher
     ([e-mail])

BUGS
     SPICE3 will recognise all the notations used in SPICE2 .plot
     cards, and will translate 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 recognised.





6






20 March 1986                                            SPICE(1)



     BJT's 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 kludge, you can set
     the variable "nobjthack", which will force BJT's 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 ._s_p_i_c_e_i_n_i_t
     file) should be a comment.  Otherwise SPICE may create an
     empty circuit structure.

CAVEATS
     SPICE3 files specified on the command line are read in
     before the .spiceinit file is read. Thus if you define
     aliases there that you call in a SPICE3 source file men-
     tioned on the command line, they won't be recognised.



































                                                                7