OP command

## 2.31 `OP` command

### 2.31.1 Syntax

`OP` start stop stepsize {options ...}

### 2.31.2 Purpose

Performs a nonlinear DC steady state analysis, with no input. If a temperature range is given, it sweeps the temperature.

### 2.31.3 Comments

There are substantial extensions beyond the capabilities of the SPICE `op` command.
If there are numeric arguments, they represent a temperature sweep. They are the start and stop temperatures in degrees Celsius, and the step size, in order. They are saved between commands, so no arguments will repeat the previous sweep.
This command will use the `op` probe set, instead of automatically printing all nodes and source currents, so you must do "`print op` ...." before running op. We did it this way because we believe that printing everything all the time is usually unnecessary clutter. All of the information available from SPICE and more is available here. See the `print` command and the device descriptions for more details.
A single parameter represents a single temperature. Two parameters instruct the computer to analyze for those two points only.
This command also sets up the quiescent point for subsequent `AC` analysis. It is necessary to do this for nonlinear circuits. The last step in the sweep determines the quiescent point for the AC analysis.

### 2.31.4 Options

`*` multiplier
  Log sweep. Multiply the absolute temperature by multiplier to get the next step. The fact that it is offset to absolute zero may make the step sizes look strange.
`>` file
  Send results of analysis to file.
`>>` file
  Append results to file.
`BY` stepsize
  Linear sweep. Add stepsize to get the next step.
`Continue`
  Use the last step of a `OP`, `DC` or `Transient` analysis as the first guess.
`Input` volts
  Apply volts input to the circuit, instead of zero.
`LOop`
  Repeat the sweep, backwards.
`PLot`
  Graphic output, when plotting is normally off.
`Print`
  Send results to printer.
`Quiet`
  Suppress console output.
`REverse`
  Sweep in the opposite direction.
`TAble`
  Tabular output. Override default plot.
`TEmperature` degrees
  Temperature, degrees C. Override the sweep.
`TImes` multiplier
  Log sweep. Multiply the absolute temperature by multiplier to get the next step.
`TRace` n
  Show extended information during solution. Must be followed by one of the following:
  `Off`
    No extended trace information (default, override .opt)
  `Warnings`
    Show extended warnings
  `Iterations`
    Show every iteration.
  `Verbose`
    Show extended diagnostics.

### 2.31.5 Examples

`op 27`
  Do a DC operating point simulation at temperature 27 degrees Celsius.
`op -50 200 25`
  Sweep the temperature from -50 to 200 in 25 degree steps. Do a DC operating point simulation at each step.
`op`
  With no parameters, it uses the same ones as the last time. In this case, from -50 to 200 in 25 degree steps.
`op 200 -50 -25`
  You can sweep downward, by asking for a negative increment.
`op Input 2.3`
  Apply an input to the circuit of 2.3 volts. This overrides the default of no input.
`op TEmperature 75`
  Simulate at 75 degrees, this time. This isn't remembered for next time.
`op`
  Since the last time used the `TEmperature` option, go back one more to find what the sweep parameters were. In this case, downward from 200 to -50 in 25 degree steps. (Because we did it 3 commands ago.)