Collection of Education

home *** CD-ROM | disk | FTP | other *** search

/ Collection of Education / collectionofeducationcarat1997.iso / SCIENCE / SPCTR3E2.ZIP / SPICE3.DOC < prev

Wrap

Text File | 1992-12-11 | 37.0 KB | 877 lines

An abridged spice3 manual, it might even be useful. This manual covers basic spice syntax and commands for using Spice TR3e2 in both interactive and batch modes. It may not be complete, but a more complete version is being worked on. SPICE (simulation program with integrated circuit emphasis) was developed in the Electronics Research Laboratory at the University of California at Berkeley. Spice3 is based on spice2. When used in batch mode, most of the syntax and commands are the same, but there are changes. For example, the output can be similar, using the -o option, or the may be written in a "RAW" file format (the raw file format must be used if it is to be plotted with Spice TR3e2's graphics capability). Polynomial non-linear sources are replaced by a General non-linear source (NOTE: most opamp libraries are made for spice2g6 and use polynomial non-linear sources-> exception: most of Linear Technology Corporation's models will work with either spice2 or spice3). Polynomial nonlinear capacitors are not supported in Spice3. *************** input format **************************** A circuit to be analyzed by Spice is described by a netlist which defines the circuit topology, element (or part) values, and may include the type of analysis to be run. Spice uses ASCII input files. The input format for Spice is of the free format type. 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 "+" in column one of the following line. Comments can be included in the listing-just place a "*" in column one of the line (a space will also work for Spice3). The first line in a Spice input file is assumed to be the circuit title. The last line must be the ".END" line. Between are the parts, type of analysis, and any subcircuits or models. The order of these statements is arbitrary (except [of course], that continuation lines must immediately follow the line being continued, and element lines belonging to a subcircuit must be between the ".SUBCKT" and ".ENDS" lines for that subcircuit). Other files may be added by using the ".include file_name" command. Spice is not case-sensitive most of the time (the ".include" command must be lower case). In Spice2, nodes must be labeled as number, in Spice3 they may be may be arbitrary character strings, except for the ground node which must be named "0". All nodes must have a dc path to ground. The circuit cannot contain a loop of voltage sources and/or inductors and cannot contain a series connection of current sources and/or capacitors. 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). Numbers may be interred directly, followed by a integer exponent, or a scale factor. 6000, 6e3, and 6k all have the same value. The scale used are: T=e12 G=e9 Meg=e6 K=e3 mil=25.4e-6 m=e-3 u=e-6 n=e-9 p=e-12 f=e-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. 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 SPICE element types is given in what follows. The strings XXXXX, YYYYY, and ZZZZZ 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. ******* Command line Usage ************ spice [ -n ] [ -b ] [ -o outfile ] [ -r rawfile ] [ input_file ] -n (or -N) Don't try to source the file "spice.rc" upon startup. Normally Spice tries to find this file in the current directory. -b (or -B) Run in batch mode. Spice will read the specified input file and do the simulation. -r rawfile (or -R rawfile) Use rawfile as the default file into which the results of the simulation are saved. If the -r option is used, the .print and .plot commands will be ignored. -o outfile (or -O outfile) Print analysis time and memory usage to a file, and if the -r option is not used, use the .print and .plot commands to make a Spice2 type output file. Further arguments are taken to be Spice input files, which are read and saved. (If batch mode is requested then they are run immediately.) Spice files specified on the command line are read in before the "spice.rc" file is read. Thus if you define aliases there, any that are used in a Spice source file mentioned on the command line won't be recognized. **************** Parts ****************************** Data fields that are enclosed in less than and greater than signs ("<" or ">") are optional. resistor Format: Rname Node1 Node2 value Examples: R1 32 45 1k rload 8 0 200 The name must start with the letter R. The value may be positive or negative, but not zero. capacitor Format: Cname Node1 Node2 value Examples: C1 32 45 1uf cload 8 0 200pf The name must start with the letter C. inductor Format: Lname +Node -Node value Examples: L1 32 45 1uh lload 8 0 200uh The name must start with the letter L. mutual inductor Format: Kname Lname1 Lname2 value Example: k1 L5 L9 .987 The name must start with the letter K. Two inductors are referenced. The standard dot convention determines polarity- with the positive node on the inductors having the dot. Value is the coefficient of coupling, which must be between 0 and 1. Lossless Transmission Lines Format: Tname N1 N2 N3 N4 Z0=value TD=value Tname N1 N2 N3 N4 Z0=value F=freq NL=nrmlen Example: t1 1 0 2 0 z0=75 td=15ns The name must start with the letter T. N1 and N2 are the nodes at port one; N3 and N4 are the nodes at port two. Z0 is the characteristic impedance. The length of the line must be expressed in either one of two forms : the delay may be specified directly (TD=value) or a frequency (F=freq) must be given. If the frequency is given, the normalized electrical length (NL=value) may be given (the default is NL=.25). NOTE1: This models only one propagating mode. If all four nodes are distinct in the actual circuit, then two modes may be excited. To simulate this, two transmission line elements are required. NOTE2: The lossy transmission line with zero loss may be more accurate due to implementation details. sources independent source Format: _name +node -node [dc value] [ac value] [tran_value] Examples: Vcc 10 0 15 Icc 2 5 1ma vin 1 0 dc 0 ac 1 pulse(-0.5 0.5 20us 20us 20us 200us 400us) If the name starts with a V it is a voltage source and if it starts with an I it is a current source. The transient value may have the following values: PULSE(v1 v2 pulse_delay [rise_time fall_time pulse_width period]) SIN(offset_voltage amplitude frequency [start_delay damping_coef]) PWL(time_point1 volt_or_amp1 [t2 v_or_a2 ...]) linear dependent sources Format: _name +nodeOut -nodeOUT +nodeIN -nodeIN value Examples: G1 10 0 5 0 15mmho E1 2 0 5 0 1e8 If the name starts with a G, it is a voltage controlled current source. If the name starts with a E, it is a voltage controlled voltage source. Format: _name +nodeOut -nodeOUT vname value Examples: F1 1 2 vz 26 H3 5 7 vy 345 Vname is the name of a voltage source through which the controlling current flows. If the name starts with a F, it is a current controlled current source. If the name starts with a H, it is a current controlled voltage source. non-linear dependent sources (these sources are not spice2 compatible) Format: Bname +nodeOut -nodeOUT <I=expr> <V=expr> Examples: b1 1 0 i=cos(v(1))+sin(v(2)) b2 5 3 v=log(v1))^2 The name must start with the letter B. The values of the V and I parameters determine the voltages and currents across and through the device, respectively. Only one of these parameters must be given. 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 following operations 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, an error will result. Other problems may arise where the partial derivative of a function is undefined. Parts that need MODELS: Some devices (or parts) that spice simulates require many parameter values. Since these devices may be used more than once in a circuit (with the same set of parameters), they have a set of "model" parameters that is defined on a separate model line with the format: .MODEL model_name type(parameters) Examples: .model mod1 npn (BF=50 IS=1e-13 VBF=50) .model dm1 d (is=2e-17) Among the model types used in Spice TR3e2bl are npn, pnp, d, njf, pjf, ltra and sw. NOTE: Although the model line is required for these parts, spice will use the default values for the unspecified parameter values. Please see some "real" spice documentation for the semiconductor default values. diodes (D) Format: Dname NodeA NodeC modname Example: d1 32 45 d1n4841 The name must start with the letter D. NodeA is the anode and NodeC is the cathode. bipolar junction transistors (NPN, PNP) Format: Qname collector base emitter modname Examples: Q1 32 45 40 Q2N2222A q27 1 2 3 q2n2222a The name must start with the letter Q. junction FETs (NJF, PJF) Format: Jname drain gate source modname Example: J1 32 45 40 JN2 The name must start with the letter J. Lossy Transmission Lines (LTRA) Format: Oname N1 N2 N3 N4 modname Example: o1 1 0 2 0 tran1 The name must start with the letter O. N1 and N2 are the nodes at port one; N3 and N4 are the nodes at port two. Note: a lossy transmission line with zero loss may be more accurate than a lossless transmission line due to implementation details. MODEL parameters R resistance/length (default 0.0) L inductance/length (default 0.0) G conductance/length (default 0.0) C capacitance/length (default 0.0) LEN length of line required -> no default REL breakpoint control (default 1) ABS breakpoint control (default 1) NOSTEPLIMIT do not limit timestep to less than time delay (flag) NOCONTROL don't do complex timestep control (flag) LININTERP use linear interpolation (flag) MIXEDINTERP use linear when quadratic seems bad (flag) COMPACTREL special reltol for history compaction COMPACTABS special abstol for history compaction TRUNCNR use Newton-Raphson method for timestep control (flag) TRUNCDONTCUT don't limit timestep to keep impulse-response errors low (flag) Only 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 RG - distributed series resistance and parallel conductance Any other combination will yield erroneous results and should not be tried. Switches (SW) Format: Sname N+ N- NC+ NC- modname <on><off> Example: s1 2 5 3 0 sw1 The name must start with the letter S (for a voltage controlled switch). Switches must always have a finite positive value. It is wise to set switch impedances only high and low enough to be negligible with respect to other circuit elements. Switches will not change state in AC analyses. MODEL parameters VT threshold voltage (default 0.0v) VH hysteresis (default 0.0v) RON on resistance (default 1 ohm) ROFF off resistance (default 1/GMIN ohm) ******************** Subcircuits ********************** A subcircuit consists of spice elements and can be referenced in a fashion similar to device models. Spice will automatically insert the group of elements wherever the subcircuit is referenced. Format for subcircuit reference: xname node1 node2 <node...> subname The name must start with the letter X. Format for subcircuit: .subckt subname sub_node1 <sub_node...> parts sub_nodes... .ends The subcircuit must end with the line: ".ends <subname>" Ground (the 0 node) may be used in a subcircuit but can not be listed as an external node. Node references in a subcircuit are independent of (not the same node as) any node which may have the same name in either the main circuit or another subcircuit. ** example of a subcircuit ** .subckt pienet 2 3 c1 2 0 100p l1 2 3 10u c2 3 0 100p .ends pienet ** end of example ** *************** Spice file commands ********************* These commands are placed in the input files for use in the batch mode, or with the interactive "run" command. dc operating point Format: .op This command directs spice3 to include the dc operating information in the RAW output file. DC analysis Format: .dc source_name vstart vstop vincrement AC analysis Format: .ac dec nd fstart fstop dec is for the decade variation, oct or lin can be used instead for the octave or linear variation. nd is the number of points per decade, octave or absolute, depending on option chosen. At least one independent source must have been specified with an ac value for the analysis to be meaningful. NOTE: AC analysis is a linear small-signal analysis. No clipping of signals will take place. Transient analysis Format: .tran tstep tstop <tstart <tmax>> Transient analysis always start at time zero, if tstart is non-zero, the data between zero and tstart is not saved. ***************** other file commands ********************** These commands are placed in the input files, all are used in the batch mode, some will not do anything in the interactive mode. Try it. If it works, it works. .NODESET V(node_number)=value V(node_number)=value ... This line may help spice 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 astable circuits, but it should not otherwise be needed. .IC V(node_number)=value V(node_number)=value ... This line is for setting transient initial conditions. It has two different interpretations, depending on whether the UIC parameter is specified on the .TRAN line. The .IC line should not be confused with the .NODESET line -> the .NODESET line does not affect final bias solution (except for multi-stable circuits). If 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 spice to compute a consistent DC solution. If the UIC parameter is specified on the .TRAN control line, 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 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. .OPTIONS option1=value option2=value ... This line allows the user to reset program control and user options for specific simulation purposes. Any combination of the following options may be included, in any order. Below, 'x' represents some positive number. option effect GMIN=x the minimum conductance allowed (default 1.0e-12) RELTOL=x the relative error tolerance (default .001 -> 0.1 percent) ABSTOL=x the absolute current error tolerance (default 1 picoamp) VNTOL=x the absolute voltage error tolerance (default 1 microvolt) CHGTOL=x the charge tolerance (default 1.0e-14) TRTOL=x the transient error tolerance (default 7) This parameter is an estimate of the factor by which spice overestimates the actual truncation error. PIVTOL=x the absolute minimum value for a matrix entry to be accepted as a pivot (default 1.0e-13) PIVREL=x the relative ratio between the largest column entry and an acceptable pivot value (default 1.0e-3) TNOM=x the nominal temperature at which device parameters are measured (default 27 deg C) TEMP=x the operating temperature of the circuit (default 27 deg C) ITL1=x the DC iteration limit (default 100) ITL2=x the DC transfer curve iteration limit (default 50) ITL3 and ITL5 are not implemented in spice3 ITL4=x the transient analysis timepoint iteration limit (default 10) METHOD=name sets the numerical integration method used by spice. possible names "Gear" or "trapezoidal" (or "trap") (default trap) .save [ node1 ] [ node2 ... ] Save a set of outputs, discarding the rest. Useful only in batch mode when a raw file format is used. If a node has been mentioned in a save command, it will appear in the raw file. If there are no save commands given, all outputs are saved. The save command must be given before an analysis command to have an affect. .print analysis_type output_var1 <output_var2 ... output_var8> .plot analysis_type output_var1 <output_var2 ... output_var8> These commands are ignored if a raw file is produced. Examples: .print ac vdb(1) db(out) .print tran v(2) i(vin) .plot tran out .four fundamental_frequency [ value ... ] This command is ignored if a raw file is produced. Does a fourier analysis of each of the given values, using the first 10 multiples of the fundamental frequency. Example: .four 10k out .include file_name Examples: .include d1n4148.mod .include ltc\lm301a ***************** interactive commands ****************** This chapter describes the most important interactive commands available for use with Spice TR3e2. It must be remembered that Spice 3e2 was written for the Unix operating system. Not all of the "Berkeley" commands will work under DR(MS)-DOS. Commands that did not work, or were considered not useful, are not listed. Those who may disagree on my definition of "what is useful" are free to call Berkeley for the "real" documentation(??). Analysis Commands: Note: While commands, in general, are not case sensitive in input files, they ARE case sensitive in the interactive mode -> use lower case. op 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. Other Commands: alias [ word ] [ text ... ] Causes word to be aliased to text. History substitutions may be used, as in C-shell aliases. cd [ directory ] Change the current working directory to directory, or to the user's home directory if none is given. destroy [ plot_name ] [ all ] Throws away the data in the named plot. This can be necessary if a lot of large simulations are being done. Spice should warn the user if the size of the memory usage is approaching the maximum allowable size (within about 90%). It is advisable to run the rusage command occasionally if running out of space is a possibility, since Spice will crash if it does runs out of memory. If the argument to destroy is all, all plots except the constant plot will be thrown away (it is not possible to destroy the constant plot). If no argument is given the current plot is destroyed. display [ vector_name ... ] 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 will be labeled [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 = []), a random remaining vector will become the scale. edit [ file ] If a filename is given, then edit that file and (when done) load it (making the circuit the current one)- else edit the current SPICE3 deck. The default editor is "VI". The "set editor=XXX" command (in either spice or DOS) can be used to select a different editor. 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). The output is like that of the .four card. 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 will be of degree polydegree if that variable is set, or 1. If polydegree is 0, then no interpolation will be done. This is likely to give erroneous results if the time scale is not monotonic, though. hardcopy file plotargs Just like plot, except creates a file containing the plot. The default file format is postscript. Other available formants are not useful under DOS. history [ number ] Print out the history, or the last number commands typed at the keyboard. Historical substitution is possible, !!<CR> will repeat the last command, !1<CR> will repeat the first command given. 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 transient 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. 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 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. load [ filename ] ... Loads the raw data from the files named. The default filename is rawspice, or the argument to the -r flag if there was one. plot exprs [ samep ] [ ylimit ylo yhi ] [ xlimit xlo xhi ] [ xindices xilo xihi ] [ xcompress comp ] [ xdelta xdel ] [ ydelta ydel ] [ xlog ] [ ylog ] [ vs xname ] [ xlabel word ] [ ylabel word ] Plot the given exprs on the screen. If samep is given, the values of the other parameters (other than xname) from the previous plot, or hardcopy command will be used unless re-defined on the command line. 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, the X or Y scale respectively will be logarithmic. The xlabel and ylabel arguments cause the specified labels to be used for the X and Y axes, respectively. 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. If the expression is all, all of the vectors available are printed. The scale vector (time, frequency) will always be in the first column unless the variable noprintscale is true. quit Quit, return to DOS. rusage [ resource ... ] Print resource usage statistics. If any resources are given, just print the usage of that resource. Currently valid resources are: elapsed The amount of time elapsed since the last rusage elapsed call. space Data space used. time CPU time used so far. everything all All of the above, and more. resume Resume a simulation after a stop (a control C will stop a run). run [ rawfile ] Run the simulation as specified in the input file. If a rawfile is given, the data is written, it is also available interactively. save [ node1 ] [ node2 ... ] 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. If there are no save commands given, all outputs are saved. The save command must be given before an analysis command to have an affect. To save the branch current through voltage source, add "source_name#branch" to the list of nodes. set [ variable ] [ variable = value ] Set the variable to value, if it is present. If no value is given then the value is the boolean 'true'. You can set a variable to be any value (numeric or string). 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 that list. Variables for Spice TR3e2: abstol The absolute tolerance used by the diff command. appendwrite Append to the file when a write command is issued, if one already exists. 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. editor The editor to use for the edit command. fourgridsize How many points to use for interpolating into when doing fourier analysis. gridsize If this variable is set to an integer, this number will be used as the number of equally spaced points to use for the Y-axis when plotting. Otherwise the current scale will be used (which may not have equally spaced points). If the current scale isn't strictly monotonic, then this option will have no effect. height The length of the page for print col. history The number of events to save in the history list. nfreqs The number of frequencies to compute in the fourier command. (Defaults to 10.) 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. nobreak Don't have print col break between pages. noclobber Don't overwrite existing files when doing IO redirection. 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 display commands), the output will be stopped every screenful and will continue when a carriage return is typed. If nomoremode is set then data will scroll off the screen without hesitation. noprintscale Don't print the scale in the leftmost column when a print col command is given. nosort Don't have display sort the variable names. numdgt The number of digits to print when printing tables of data (fourier, print col). The default precision is 6 digits. Approximately 16 decimal digits are available, so numdgt should not be more than 16. If the number is negative, one fewer digit is printed to ensure constant widths in tables. polydegree The degree of the polynomial that the plot command should fit to the data. If polydegree is N, then nutmeg will fit 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 will try 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. (This should really be done automatically.) prompt The prompt, with the character `!' replaced by the current event number. rawfile The default name for rawfiles created. rawfileprec The number of digits to use in the ascii rawfile format. The default is 15. reltol The relative tolerance used by the diff command. sourcepath A list of the directories to search when a source command is given. The default is the current directory and the SPICE_PATH\scripts. units If this is degrees, then all the trig functions will use degrees instead of radians. unixcom When this variable is set, Spice will try to "shell" any non-spice command. vntol The absolute voltage tolerance used by the diff command. width The width of the page for print col. 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 "source" command (see below) it becomes the current circuit. 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 will become one with no vectors defined. Note that here the word "plot" refers to a group of vectors that are the result of one SPICE run. When more than one file is loaded in, or more than one plot is present in one file, they are keep separate and only the vectors in the current plot can be plotted. shell [ args ... ] Fork a shell, or execute the arguments as a command to DOS. If the "set unixcom" command is used (as it is in the default spice.rc file), Spice will try to "shell" any non-spice command that it can not "source". show device Show a device's parameters. source file Read the Spice input file file. Interactive Spice commands may be included in the file, but they must be enclosed between the lines ".control" and ".endc" (the file "spice.rc" which is read on startup does not need these two lines). These commands are executed immediately after the circuit is loaded. Spice3 command scripts, other than spice.rc, must begin with a blank or title line. Also, any line beginning with the characters "*#" will be executed as a command. The use of this command is some what unnecessary, since Spice will try to "source" any non-spice command. unalias [ word ... ] Removes any aliases present for the words. unset [ word ] ... Unset the variables word. version [ version_id ] displays the version of Spice that is running. If there are arguments, it checks to make sure that the arguments match the current version of Spice. This is mainly used as a command line in rawfiles. where Gives the name of the last node or device to cause non-convergence (for transient and operating point analysis). Note: only one node or device is printed- there may be more than one problem. write [ file ] [ exprs ... ] Writes the expr's to file. First vectors are grouped together by plots, and written out as such. Additionally, if the scale for a vector isn't present, it is automatically written out as well. 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.