The commands described in this section initiate, control, and monitor WRspice simulations. One can monitor the progress of a run in two ways, in addition to the percentage complete that is printed in the Tool Control window. First, the iplot command can be used to plot one or more variables as the simulation is progressing. To plot v(1), for example, one would type, before the run is started, ``iplot v(1)''. During the run, v(1) will be plotted on screen, with the plot rescaled as necessary. Second, one can print variables. For example, the trace command can be used, by typing ``trace time'' before the run starts, to cause the time value to be printed at each output point during transient analysis.
The iplot and trace commands are examples of what are called ``runops''. Other runops include the stop and measure commands. A runop remains in effect until deleted with the delete command, and the runops in effect can be listed with the status command. The runops can also be listed, deleted, or made inactive with the Trace tool from the Tools menu in the Tool Control window. All runops are available as commands, which apply to any circuit while in force. Some runops can be specified from within the WRspice input file, in which case the runop applies when simulating that file only. The table below lists the runops that are presently available.
The run can be paused at any time by typing Ctrl-C in the controlling text window. The run can be resumed with the resume command, or reset with the reset command.
It is possible to transparently execute simulations on a remote machine while in WRspice, if the remote machine has a wrspiced daemon running. It is also possible to run simulations asynchronously on the present machine. These jobs are not available for use with the iplot command, however. The jobs command can be used to monitor their status.
Many of these commands operate on the ``current circuit'' which by default is the last circuit entered into WRspice explicitly with the source command, or implicitly by typing the file name. The setcirc command can be used to change the current circuit. The Circuits button in the Tools menu also allows setting of the current circuit.
When a circuit file is read, any references to shell variables are expanded to their definitions. Shell variables are referenced as $name, where name has been set with the set command or in the .options line. This expansion occurs only when the file is sourced, or the reset command is given, so that if the variable is changed, the circuit must be sourced or reset to make the change evident in the circuit. If a variable is set in the shell and also in the .options line, the value from the shell is used.
|ac||Perform ac analysis|
|alter||Change circuit parameter|
|alterf||Dump alter list to Monte Carlo output file|
|aspice||Initiate asynchronous run|
|cache||Manipulate subcircuit/model cache|
|check||Initiate range analysis|
|dc||Initiate dc analysis|
|devcnt||Print device counts|
|devload||Load device module|
|devls||List available devices|
|devmod||Change device model levels|
|disto||Initiate distortion analysis|
|dump||Print circuit matrix|
|findlower||Find lower edge of operating range|
|findrange||Find edges of operating range|
|findupper||Find upper edge of operating range|
|free||Delete circuits and/or plots|
|jobs||Check asynchronous jobs|
|loop||Alias for sweep command|
|mctrial||Run a Monte Carlo trial|
|measure||Set up a measurement|
|noise||Initiate noise analysis|
|op||Compute operating point|
|pz||Initiate pole-zero analysis|
|resume||Resume run in progress|
|rhost||Identify remote SPICE host|
|rspice||Initiate remote SPICE run|
|save||List vectors to save during run|
|sens||Initiate sensitivity analysis|
|setcirc||Set current circuit|
|state||Print circuit state|
|status||Print trace status|
|stop||Specify stop condition|
|sweep||Perform analysis over parameter range|
|tf||Initiate transfer function analysis|
|tran||Initiate transient analysis|
|vastep||Advance Verilog simulator|
|where||Print nonconvergence information|