Command Line Interface

Multisim Help


Edition Date: February 2017
Part Number: 375482B-01
View Product Info

DOWNLOAD (Windows Only)


Multisim 14.0 and 14.0.1 Help
Multisim 14.1 Help
Multisim 14.2 Help

The Command Line Interface enables you to perform simulations by typing commands instead of using schematic capture or the analysis dialogs.

To open the Command Line Interface, choose Simulate»XSPICE command line interface. The XSPICE Command Line dialog box appears.

The Command Line Interface is used from within the Multisim environment; it may not be used from the operating system's command prompt.

  In many cases it may be more convenient to use the User-Defined Analysis as this allows you to run the commands in batched form. Refer to the User-Defined Analyses section for information. Another convenient alternative is to use the Arbitrary SPICE Block component from the Multsim component database. This component allows you to add SPICE code directly into the netlist. Refer to the Component Help for information.

The Command Line Interface supports a vast array of commands most of which are beyond the scope of this document. In the command line, type "help all" to get more information. Described below is a set of the most common commands.

  • source <PATH>
  • Loads a netlist from a file into the simulator.

    <PATH> the full path to the netlist.

    Example:

    source c:\sim\filter.cir

  • op
  • Performs a DC Operating Point Analysis. The command has no arguments.

  • ac <sweep type> <Nsteps> <StartFreq> <EndFreq>
  • Performs an AC sweep analysis.

    <sweep type> oct, dec, or lin.

    <Nsteps>    for octave and decade sweeps, this is the number of frequency steps per octave and per decade, whichever applies. For linear sweep, this is the total number of frequency steps.

    <StartFreq> starting frequency.

    <EndFreq>   ending frequency.

    Example:

    ac dec 10 0.1 100k

  • tran <TSTEP> <TSTOP> <TSTART><TMAX><UIC>
  • Performs an a transient (time-domain) analysis.

    <TSTEP> initial step size.

    <TSTOP> analysis end time.

    <TSTART> data recording start time.

    <TMAX> maximum step size allowed.

    <UIC> user-defined initial conditions flag (optional).

    Example:

    tran 1u 5m 0 1u uic

  • dc <Source1> <StartVal1> <EndVal1> <StepSize1> <Source2> <StartVal2> <EndVal2> <StepSize2>
  • Performs a DC Operating Point Sweep analysis.

    <Source1>   voltage or current source to sweep.

    <StartVal1> starting value for Source1.

    <EndVal1>   ending value for Source.

    <StepSize1> size of the step.

    <Source2>   voltage or current source to sweep (optional).

    <StartVal2> starting value for Source1 (optional).

    <EndVal2>   ending value for Source1 (optional).

    <StepSize2> size of the step for Source1 (optional).

  • plot <variable1> <variable2>...<variableN>
  • Plots the simulation result in the grapher.

    <variableX> the circuit variable to be plotted. Use V(node) for voltage nodes and SourceName#branch for voltage source branch currents.

    Example:

    plot v(15,16) vin#branch

  • set <options>
  • Sets the internal simulator options.

    <options>  A list of simulator options and their assignments

    Example:

    set retol=0.01

WAS THIS ARTICLE HELPFUL?

Not Helpful