1SPICE(1) General Commands Manual SPICE(1)
2
6 spice - circuit simulator
7
9 spice [ -n ] [ -t term ] [ -r rawfile] [ -b ] [ -i ] [ input file ... ]
10
12 This manual page describes the commands available for interactive use
13 of SPICE3. For details of circuit descriptions and the process of simu‐
14 lating a circuit, see the SPICE3 User's Manual. The commands available
15 are a superset of those available for nutmeg - only the additional com‐
16 mands available in SPICE3 are described here. You should be familiar
17 with the manual page for nutmeg(1) before reading this manual page.
18 Arguments are:
20 -n (or --no-spiceinit)
22 Don't try to source the file ".spiceinit" upon startup. Normally
23 SPICE3 tries to find the file in the current directory, and if
24 it is not found then in the user's home directory.
25 -q (or --completion)
27 Enable command completion.
28 -t term (or --term=term)
30 The program is being run on a terminal with mfb name term.
31 -b (or --batch)
33 Run in batch mode. SPICE3 will read the standard input or the
34 specified input file and do the simulation. Note that if the
35 standard input is not a terminal, SPICE3 will default to batch
36 mode, unless the -i flag is given.
37 -s (or --server)
39 Run in server mode. This is like batch mode, except that a tem‐
40 porary rawfile is used and then written to the standard output,
41 preceded by a line with a single "@", after the simulation is
42 done. This mode is used by the spice daemon.
43 -i (or --interactive)
45 Run in interactive mode. This is useful if the standard input is
46 not a terminal but interactive mode is desired. Command comple‐
47 tion is not available unless the standard input is a terminal,
48 however.
49 -r rawfile (or --rawfile=file)
51 Use rawfile as the default file into which the results of the
52 simulation are saved.
53 -c circuitfile (or --circuitfile=circuitfile)
55 Use circuitfile as the default input deck.
56 -h (or --help)
58 Display a verbose help on the arguments available to the pro‐
59 gram.
60 -v (or --version)
62 Display a version number and copyright information of the pro‐
63 gram.
64 Further arguments are taken to be SPICE3 input decks, which are read
66 and saved. (If batch mode is requested then they are run immediately.)
67 SPICE3 will accept any SPICE2 input decks, and output ascii plots,
69 fourier analyses, and node printouts as specified in .plot, .four, and
70 .print cards. If a out parameter is given on a .width card, the effect
71 is the same as set width = .... Since SPICE3 ascii plots do not use
72 multiple ranges, however, if vectors together on a .plot card have dif‐
73 ferent ranges they will not provide as much information as they would
74 in SPICE2. The output of SPICE3 is also much less verbose than SPICE2,
75 in that the only data printed is that requested by the above cards.
76 Vector names are the same as in nutmeg, with this addition: a name such
78 as @name[param], where name is either the name of a device instance or
79 model, denotes the value of the param parameter of the device or model.
80 See the SPICE3 User's Manual for details of what parameters are avail‐
81 able. The value is a vector of length 1. This function is also avail‐
82 able with the show command, and is available with variables for conve‐
83 nience for command scripts.
84 SPICE3 commands are as follows (these are only those commands not also
86 available in nutmeg - consult the nutmeg manual page for more com‐
87 mands):
88 setcirc [circuit name]
90 Change the current circuit. The current circuit is the one that
91 is used for the simulation commands below. When a circuit is
92 loaded with the source command (see below) it becomes the cur‐
93 rent circuit.
94 op [.op card args]
96 Do an operating point analysis.
97 tran [.tran card args]
99 Do a transient analysis.
100 ac [.ac card args]
102 Do an ac analysis.
103 dc [.dc card args]
105 Do a dc transfer curve analysis.
106 listing [logical] [physical] [deck] [expand]
108 Print a listing of the current circuit. If the logical argument
109 is given, the listing is with all continuation lines collapsed
110 into one line, and if the physical argument is given the lines
111 are printed out as they were found in the file. The default is
112 logical. A deck listing is just like the physical listing,
113 except without the line numbers it recreates the input file ver‐
114 batim (except that it does not preserve case). If the word
115 expand is present, the circuit will be printed with all subcir‐
116 cuits expanded.
117 edit [file]
119 Print the current SPICE3 deck into a file, call up the editor on
120 that file and allow the user to modify it, and then read it back
121 in, replacing the origonal deck. If a filename is given, then
122 edit that file and load it, making the circuit the current one.
123 resume Resume a simulation after a stop.
125 show Show a device parameter.
127 alter Alter a device parameter.
129 state Print the state of the circuit. (This command is largely unim‐
131 plemented.)
132 save [all] [output ...] or .save [all] [output ...]
134 Save a set of outputs, discarding the rest. If a node has been
135 mentioned in a save command, it will appear in the working plot
136 after a run has completed, or in the rawfile if spice is run in
137 batch mode. If a node is traced or plotted (see below) it will
138 also be saved. For backward compatibility, if there are no save
139 commands given, all outputs are saved.
140 stop [ after n] [ when something cond something ] ...
142 Set a breakpoint. The argument after n means stop after n itera‐
143 tion number n, and the argument when something cond something
144 means stop when the first something is in the given relation
145 with the second something, the possible relations being eq or =
146 (equal to), ne or <> (not equal to), gt or > (greater than), lt
147 or < (less than), ge or >= (greater than or equal to), and le or
148 <= (less than or equal to). IO redirection is disabled for the
149 stop command, since the relational operations conflict with it
150 (it doesn't produce any output anyway). The somethings above
151 may be node names in the running circuit, or real values. If
152 more than one condition is given, e.g. stop after 4 when v(1) >
153 4 when v(2) < 2, the conjunction of the conditions is implied.
154 trace [ node ...]
156 Trace nodes. Every iteration the value of the node is printed to
157 the standard output.
158 iplot [ node ...]
160 Incrementally plot the values of the nodes while SPICE3 runs.
161 step [number]
163 Iterate number times, or once, and then stop.
164 status Display all of the traces and breakpoints currently in effect.
166 delete [debug number ...]
168 Delete the specified breakpoints and traces. The debug numbers
169 are those shown by the status command. (Unless you do status >
170 file, in which case the debug numbers aren't printed.)
171 reset Throw out any intermediate data in the circuit (e.g, after a
173 breakpoint or after one or more analyses have been done
174 already), and re-parse the deck. The circuit can then be re-run.
175 (Note: this command used to be end in SPICE 3a5 and earlier ver‐
176 sions -- end is now used for control structures.) The run com‐
177 mand will take care of this automatically, so this command
178 should not be necessary...
179 run [rawfile]
181 Run the simulation as specified in the input file. If there were
182 any of the control cards .ac, .op, .tran, or .dc, they are exe‐
183 cuted. The output is put in rawfile if it was given, in addition
184 to being available interactively.
185 source file
187 Read the SPICE3 input file file. Nutmeg and SPICE3 commands may
188 be included in the file, and must be enclosed between the lines
189 .control and .endc. These commands are executed immediately
190 after the circuit is loaded, so a control line of ac ... will
191 work the same as the corresponding .ac card. The first line in
192 any input file is considered a title line and not parsed but
193 kept as the name of the circuit. The exception to this rule is
194 the file .spiceinit. Thus, a SPICE3 command script must begin
195 with a blank line and then with a .control line. Also, any line
196 beginning with the characters *# is considered a control line.
197 This makes it possible to imbed commands in SPICE3 input files
198 that will be ignored by earlier versions of SPICE. Note: in
199 spice3a7 and before, the .control and .endc lines were not
200 needed, and any line beginning with the name of a front-end com‐
201 mand would be executed.
202 linearize vec ...
204 Create a new plot with all of the vectors in the current plot,
205 or only those mentioned if arguments are given. The new vectors
206 will be interpolated onto a linear time scale, which is deter‐
207 mined by the values of tstep, tstart, and tstop in the currently
208 active transient analysis. The currently loaded deck must
209 include a transient analysis (a tran command may be run interac‐
210 tively before the last reset, alternately), and the current plot
211 must be from this transient analysis. This command is needed
212 because SPICE3 doesn't output the results from a transient anal‐
213 ysis in the same manner that SPICE2 did.
214 There are several set variables that SPICE3 uses but nutmeg does not.
216 They are:
217 editor
219 The editor to use for the edit command.
220 modelcard
222 The name of the model card (normally .model).
223 noaskquit
225 Do not check to make sure that there are no circuits
226 suspended and no plots unsaved. Normally SPICE3 will
227 warn the user when he tries to quit if this is the
228 case.
229 nobjthack
231 Assume that BJT's have 4 nodes.
232 noparse
234 Don't attempt to parse decks when they are read in
235 (useful for debugging). Of course, they cannot be run
236 if they are not parsed.
237 nosubckt
239 Don't expand subcircuits.
240 renumber
242 Renumber input lines when a deck has .include's.
243 subend
245 The card to end subcircuits (normally .ends).
246 subinvoke
248 The prefix to invoke subcircuits (normally x).
249 substart
251 The card to begin subcircuits (normally .subckt).
252 There are a number of rusage parameters available, in addition to the
254 ones available in nutmeg:
255 If there are subcircuits in the input file, SPICE3 expands instances of
259 them. A subcircuit is delimited by the cards .subckt and .ends, or
260 whatever the value of the variables substart and subend is, respec‐
261 tively. An instance of a subcircuit is created by specifying a device
262 with type 'x' - the device line is written
263 xname node1 node2 ... subcktname
265 where the nodes are the node names that replace the formal parameters
267 on the .subckt line. All nodes that are not formal parameters are
268 prepended with the name given to the instance and a ':', as are the
269 names of the devices in the subcircuit. If there are several nested
270 subcircuits, node and device names look like subckt1:subckt2:...:name.
271 If the variable subinvoke is set, then it is used as the prefix that
272 specifies instances of subcircuits, instead of 'x'.
273
275 The standard suffix for rawspice files in VMS is ".raw".
276 You may have to redefine the value EDITOR if you wish to use the edit
278 command, since the default for VMS is "vi".
279
281 nutmeg(1), sconvert(1), spice(1), mfb(3), writedata(3) SPICE3 User's
282 Guide
283
285 SPICE3: Tom Quarles (quarles@cad.berkeley.edu)
286 nutmeg / User interface: Wayne Christopher (faustus@cad.berkeley.edu)
287
289 SPICE3 will recognise all the notations used in SPICE2 .plot cards, and
290 will translate vp(1) into ph(v(1)), and so forth. However, if there are
291 spaces in these names it won't work. Hence v(1, 2) and (-.5, .5) aren't
292 recognised.
293 BJT's can have either 3 or 4 nodes, which makes it difficult for the
295 subcircuit expansion routines to decide what to rename. If the fourth
296 parameter has been declared as a model name, then it is assumed that
297 there are 3 nodes, otherwise it is considered a node. To disable this
298 kludge, you can set the variable "nobjthack", which will force BJT's to
299 have 4 nodes (for the purposes of subcircuit expansion, at least).
300 The @name[param] notation might not work with trace, iplot, etc. yet.
302 The first line of a command file (except for the .spiceinit file)
304 should be a comment. Otherwise SPICE may create an empty circuit
305 structure.
306
308 SPICE3 files specified on the command line are read in before the .spi‐
309 ceinit file is read. Thus if you define aliases there that you call in
310 a SPICE3 source file mentioned on the command line, they won't be
311 recognised.
3124th Berkeley Distribution 20 March 1986 SPICE(1)