TclSpice - Manuals - Interactive commands (original) (raw)

spice::ac

Perform an AC, small-signal frequency response analysis.

 spice::ac [ DEC | OCT | LIN ] N Fstart Fstop

Do an ac analysis.

spice::alias

Create an alias for a command.

 spice::alias [ word ] [ text ... ]

Causes word to be aliased to text.

spice::alter

Change a device or model parameter.

 spice::alter dev = expression
 spice::alter dev param = expression
 spice::alter @dev[param] = expression

General form [pre 3f4]:

 spice::alter device value
 spice::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.) the other forms are 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 "]".

spice::altermod

[Note: Altermod is absent from many implemetations, use alter instead.]

spice::asciiplot

Plot values using old-style character plots.

spice::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.

spice::aspice

Asynchronous Spice run.

spice::aspice input-file [ output-file ]

Start a Spice-3 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.

spice::bg

Run spice commands in the background.

spice::bg run
spice::bg resume

All spice commands should be recognised.

spice::bltplot

spice::break

Control structure.

spice::break

If there is a while, dowhile, or foreach 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.

spice::bug

Mail a bug report.

spice::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 Spice that you are running, and the relevant Spice input file.

spice::cd

Change directory.

spice::cd [ directory ]

Change the current working directory to directory, or to the user's home directory if none is given.

spice::cdump

spice::compose

Compose a vector.

 spice::compose name values value1 [ value2 ... ]
 spice::compose name parm = val [ parm = val ... ]

[Note: This command was not fully implemented in the Berkeley release, however it is a way to create a vector from a list of values, which is lucky because the Berkeley frontend parser rejects expressions like [ 11 22 33 ].]

The first form takes the values and creates a new vector, the values may be arbitrary expressions.

The second form has the following possible parameters:

start	The value at which the vector should start.
stop	The value at which the vector should end.
step	The difference between sucessive elements.
lin	The number of points, linearly spaced.
log	The number of points, logarithmically spaced.
dec	The number of points per decade, logarithmically spaced.
center	Where to center the range of points.
span	The size of the range of points.

spice::continue

Control structure.

spice::continue

If there is a while, dowhile, or foreach enclosing this statement, control passes out to the test, or in the case of foreach, the next value is taken. Otherwise an error results.

spice::cross

Create a vector.

spice::cross vecname n [ vector1 vector2 ... ]

Create a new vector vecname from the nth elements of the listed vectors. Note: If any input vector is complex then the output vector will be complex, and vector[n] is the first element of vector. If n is a vector only the real part of its first element is used.

spice::dc

Perform a DC-sweep analysis.

spice::dc Source-Name Vstart Vstop Vincr [ Source2 Vstart2 Vstop2 Vincr2 ]

Do a dc transfer curve analysis.

spice::define

Define a function.

     spice::define function(arg1 [ , arg2  ... ]) expression

Define the user-definable function with the namefunction 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 [i.e. number of arguments.].

Some useful definitions are:

    define max(x,y) (x > y) * x + (x <= y) * y
define min(x,y) (x < y) * x + (x >= y) * y

spice::deftype

Define type of plot or vector.

spice::deftype spec name pan

Redefine vector and plot types.

spice::delete

Remove a trace or breakpoint.

spice::delete [ debug-number ... ]

Delete the specified breakpoints, traces and saves. The debug numbers are those shown by the status command (unless you do status > file, in which case the debug numbers are not printed).

spice::delta

set Delta value.

spice::delta value

Sets the value of delta to the given value, if given. It returns the current setting of delta

spice::destroy

Delete a data set.

spice::destroy [ plotnames | all ]

Release the memory holding the data for the specified runs.

spice::diff

Compare vectors.

spice::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 what is meant by a significant difference.

spice::display

List known vectors and types.

spice::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 labeled [scale]. When a command such asplot 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). See also setscale.

spice::disto

spice::dowhile

Control structure.

 spice::dowhile condition
                statement
                ...
 spice::end

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

spice::dump

spice::echo

Print text.

spice::echo [ -n ] [ text ... ]

Echos the given text to the screen. If the first argument is -n the terminating newline is suppressed.

spice::edit

Edit the current circuit.

spice::edit [ file ]

Print the current Spice3 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.

spice::else

Control structure.

 spice::if condition
           statement
           ...
 spice::else
           statement
           ...
 spice::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.

spice::end

Control structure.

spice::end

Terminates if, while, dowhile and foreach control structures

spice::foreach

Control structure.

 spice::foreach var value ...
              statement
              ...
 spice::end

The statements are executed once for each of thevalues, each time with the variable var set to the current one. (var can be accessed by the $var notation - see below).

spice::fourier

Perform a fourier transform.

spice::fourier fundamental [ 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 Spice3 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 degreepolydegree 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.

spice::get_output

spice::get_param

spice::goto

Control structure.

spice::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).

spice::halt

Interrupts a simualtion.

spice::halt

spice::hardcopy

Save a plot to a file for printing.

spice::hardcopy file plotargs

Just like plot, except creates a file called file containing the plot in the format specified by the variable hcopydevtype. The default file format is an image in plot(5) format, and can be printed by either the [unix] plot(1) program or lpr with the -g flag. See also the hcopy variables.

spice::help

Print summaries of Spice3 commands.

spice::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.

spice::history

Review previous commands.

spice::history [ -r ] [ number ]

Print out the history, or the last number commands typed at the keyboard. Note: in Spice3 version 3a7 and earlier, all commands (including ones read from files) were saved. The -r option reverses the printing order

spice::if

Control structure.

 spice::if condition
           statement
           ...
 spice::else
           statement
           ...
 spice::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.

spice::iplot

Incremental plot.

spice::iplot [ node ... ]

Incrementally plot the values of the nodes while Spice3 runs. The iplot command can be used with thewhere command to find trouble spots in a transient simulation; it is essentially a graphical version of trace. Several iplots may be active simulataneously. Iplotting is not applicable for all analyses. The status command displays a list of current iplots, and these can be removed with the delete command.

spice::jobs

List active asynchronous Spicer runs.

spice::jobs

Report on the asynchronous Spice-3 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.

spice::label

Control structure.

spice::label word

If a statement of the form goto word is encountered, control is transferred to this point, otherwise this is a no-op.

spice::lastvector

Save vectors last values.

spice::lastvector bltVectorName

Sets bltvectorName with all the vectors values at the last timestep.

spice::let

Assign a value to a vector.

spice::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 [Note: This doesn't work with the Berkeley 3f4/5 release code, try unlet instead.]. Individual elements of a vector may be modified by appending a subscript to name (e.g. name[0]). If there are no arguments, let is the same as display.

[Note. Let creates a vector in the current plot, use set to create a new plot.]

spice::linearize

Interploate to a linear scale.

spice::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 Spice3 doesn't output the results from a transient analysis in the same manner that Spice2 did.

spice::listTriggers

Lists all set triggers.

spice::listtriggers

Returns a list of triggers set by registerTriggers.

spice::listings

Print a listing of the current circuit.

spice::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.

spice::load

Load rawfile data.

spice::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 when Spice was invoked.

spice::loadsnap

***

spice::loadsnap inputfile snapFileName

***

spice::maxstep

Maximum step size allowed.

spice::maxstep stepsize

Same as delta but for the maximum stepsize allowed.

spice::newhelp

spice::noise

Perform a noise analysis.

spice::noise v(output [,ref) src [ DEC | LIN | OCT ] Pts Fstart Fstop [PPS]

Do an noise analysis.

spice::oldhelp

spice::op

Perform an operating point analysis.

spice::op

Do a operating point analysis.

spice::option

spice::plot

Plot values on the display.

 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]
      [keyword ... ]

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. Thexindices arguments determine what range of points are to be plotted - everything between the xiloth point and the xihith 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 ydelrespectively.

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 asciiplotcommand 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 following keywords are available in Spice3f:

linear	override a default log-scale plot (as in the output for an AC analysis
linplot	synonym for linear
lingrid	override a default log-scale plot without tranforming the data
smith	Smith plot - data is transformed by the function (x-1)/(x+1)
gridsmith	polar plot with a Smith grid but without transforming the data.
pointplot	plot the points without joining them.
combplot	plot vectors by drawing a vertical line from each point to the X-axis, as opposed to joining the points.

[Note: The Berkeley release version of this command seems to ignore the variables that one would expect to influence this command. CDHW.]

spice::plot_datapoints

Time steps.

spice::plot_datapoints plot

returns number of time steps saved so far.

spice::plot_data

Returns date string.

spice::plot_date plot

spice::plot_get_value

Returns value of varable "name" in plot "plot", at position "index".

spice::plot_get_value name plot index

spice::plot_name

Returns plot name.

spice::plot_name plot

spice::plot_nvars

Returns number of variables in the plot.

spice::plot_nvars plot

spice::plot_title

Returns plot title.

spice::plot_title plot

spice::plot_variables

Returns a list of variables in plot "plot" plot is from 0-numofplots, newest plot being 0.

spice::plot_variables plot

spice::popTriggerEvents

***

spice::popTriggerEvent

***pops the stack of saved triggers returning { Node ? ? ? }

spice::print

Print values.

spice::print [ col ] [ line ] expr [ expr2 ... ]

Prints the vector described by the expression expr. If thecol 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,height, 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.

spice::pz

Pole-Zero Analysis.

spice::pz node1 node2 node3 node4 { CUR | VOL } { POL | ZER | PZ }

Performs a pole-zero analysis of the current circuit, as described earlier.

spice::quit

Leave Spice3 or Nutmeg.

spice::quit

Quit nutmeg or Spice.

spice::registerTriggers

***

spice::registerTriggers node start** finish***

***

spice::rehash

Reset internal hash tables.

spice::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

spice::repeat

 spice::repeat [ number ]
                statement
                ...
 spice::end

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

spice::reset

Reset an analysis.

spice::reset

spice::reshape

Alter the dimensionality or dimensions of a vector.

 spice::reshape vector vector ...
 or
 spice::reshape vector vector ...  [ dimension, dimension, ...  ]
 or
 spice::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 xwere inconsistent' can be ignored.

spice::resume

Continue a simulation after a stop.

spice::resume

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

spice::rspice

Remote Spice submission.

spice::rspice input file

Runs a Spice-3 remotely taking the input file as a Spice-3 input file, or the current circuit if no argument is given. Nutmeg or Spice3 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 Spice3 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. [Note: Altermod is absent from many implemetations, use alter instead.]

spice::run

Run analysis from the input file.

spice::run [ rawfile ]

Run the analyses specified in the input file for the current circuit. If there are any of the control lines specified in Section 4.3 present they are executed. The output is put in rawfile if it is 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 effect.

spice::running

Simulation state.

spice::running

Returns a '1' if simultaion is running, else a '0' if simulation has been interupted or halted.

spice::rusage

Resource usage.

spice::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:

all	Everything below.
elapsed	The amount of time elapsed since the last rusage elaped 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 (listed incorrectly as "Transient iterations per point")
tranlutime	Transient L-U decomposition time
transolvetime	Transient matrix solve time

everything	All of the above.

spice::save

Save a set of outputs.

spice::save [ all | 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 Spice is run in batch mode. If a node istraced 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" appears in the save command, all default values (node voltages and voltage source currents) are saved in addition to any other values listed. See also the status command.

spice::savesnap

***

spice::savesnap filename

***see also loadsnap

spice::sens

Run a sensitivity analysis.

 spice::sens output
 spice::sens output ac [ DEC | OCT | LIN ] N Fstart Fstop

Perform a sensitivity analysis. The variable output is either a node voltage (e.g. "v(1)" or "v(A,out)") or a current through a voltage source (e.g. "i(vtest)"). The first form calculates DC sensitivities, the second form calculates AC sensitivities. 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).

spice::set

Set the value of a variable.

 spice::set [ word ]
 spice::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 affecting Nutmeg are listed in the following section (5.5). The 'set' command can also be used to change simulator parametersfor the current circuit (see setcirc below). Set values will be used (until the circuit is reset) when the current circuit isrun and take precedence over a .options statement.

spice::setcirc

Change the current circuit.

 spice::setcirc [ cktname ]

Selects cktname as the 'current' circuit. When a circuit is loaded with the source command it is added to a list of available circuits and becomes the current circuit. The setcirc without an argument prints a menu of available circuits.

spice::setplot

Switch the current set of vectors.

 spice::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, above.) 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 Spice analysis 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.

spice::setscale

Set the scale vector for current plot.

 spice::setscale [ vector ]

Defines the scale vector for the current plot. If no argument is given, the current scale vector is printed.

spice::settype

Set the type of a vector.

 spice::settype type vector [ vector ... ]

Change the type of the named vectors to type. Type names can be found in the manual page for sconvert.

spice::shell

Call the command interpreter.

 spice::shell [ command ]

Call the operating system's command interpreter; execute the specified command or call for interactive use.

spice::shift

Alter a list variable.

 spice::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 isargv, and the default number is 1.

spice::show

List device state.

 spice::show devices [ : parameters ] , ...

Old form:

 spice::show -v @device [ [ name ] ]

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 parameterscontains 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.

The "old form" (with "-v") prints the data in an older, more verbose pre-Spice3f format.

spice::showmod

List model parameter values.

 spice::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".

spice::source

Read a Spice3 input file.

 spice::source file

For Spice3: Read the Spice3 input file file. Nutmeg and Spice3 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 Spice3 command script must begin with a blank line and then a control line. Also, any line starting with the characters *# is considered a control line. This makes it possible to embed commands in Spice3 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.

spice::spec

Create a frequency domain plot.

 spice::spec start_freq stop_freq step_freq vector [vector ...]

Calculates a new complex vector containing the Fourier transform of the input vector (typically the linearized result of a transient analysis). The default behaviour is to use a Hanning window, but this can be changed by setting the variables specwindow and specwindoworderappropriately. Typical usage:

spice3 > [linearize](#linearize)
spice3 > [set](#set) specwindow = "blackman"
spice3 > spec 10 1000000 1000 v(out)
spice3 > [plot](#plot) mag(v(out))

Possible values for specwindow are: none, hanning,cosine, rectangular, hamming, triangle,bartlet, blackman, gaussian. In the case of a gaussian window specwindoworder is a number specifying its order.

[Note: This command was not part of the original Berkeley Spice release. The source code was released by its author, and is often incorporated. A command script version is (Hanning window only) available for use in other cases.

spice::spice

Foreground run.

spice::spice command

Runs the specified spice command in the foreground.

spice::spice_data

List spice variables.

spice::spice_data

Returns the names and types of avaliable spice variables {name type} {name type} ... {name type}.

spice::spice_header

File header information.

spice::spice_header

Returns the current run's title, analysis name, date, and the number of signals as follows: {title ??} {name ???} {date ????} {variables ???}.

spice::spicetoblt

Assign node values to a BLT vector.

spice::spicetoblt node bltVectorName [ startStep ] [ endStep ]

Sets bltVectorName with all node values from startStep to endstep.

spice::state

lists simultaion information.

spice::state

*****

spice::status

Display breakpoint information.

 spice::status
 spice::status > file

Display all of the save, trace, iplot and breakpoint events currently in effect. If the output is redirected to a file, it is assumed that the intention is to re-import it later using the source command so the event numbers are omitted.See also thedelete command.

spice::step

Run a fixed number of timepoints.

 spice::step [ number ]

Iterate number times, or once, and then stop.

spice::stop

Set a breakpoint.

 spice::stop [ after n ] [ when value cond value ] ...

Set a breakpoint. The argument 'after n' means stop after 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

gt >	lt <	ge >=
le <=	ne <>	eq =

IO redirection is disabled for the stop command, since the relational operations conflict with it (stop 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.

0	if they are equal
Negative integer	if str1 < str2
Positive integer	if str1 > str2