http://ltwiki.org/api.php?action=feedcontributions&user=Rsfjr&feedformat=atomLTwiki-Wiki for LTspice - User contributions [en]2024-03-29T01:17:04ZUser contributionsMediaWiki 1.31.7http://ltwiki.org/index.php?title=Simulation_Command&diff=1283Simulation Command2014-01-29T21:06:13Z<p>Rsfjr: </p>
<hr />
<div>At the netlist level the '''Simulation Command''' is simply a line of text that begins with any of the following Dot Commands:<br />
.tran <Tstep> <Tstop> [Tstart [dTmax]] [modifiers]<br />
.ac <oct, dec, lin> <Nsteps> <StartFreq> <EndFreq><br />
.dc <srcnam> <Vstart> <Vstop> <Vincr> [<srcnam2> <Vstart2> <Vstop2> <Vincr2>]<br />
.noise V(<out>[,&lt;ref>]) <src> <oct, dec, lin> <Nsteps> <StartFreq> <EndFreq><br />
.tf V(<node>[, &lt;ref>]) <source> '''''OR''''' I(<voltage source>) <source><br />
.op<br />
At the schematic level these commands may be entered directly as a [[SPICE Directive]] (''ctrl''-right-click on the text to edit) or may be entered via the drop down menu item: '''Simulate => Edit Simulation Cmd'''.<br />
<br />
The '''Edit Simulation Command''' dialog box organized like a row of tabbed index cards:<br />
<br />
{|table width="400" cellspacing="0" border="1" style="background-color: #DDDDDD"<br />
|- align="center"<br />
| [[#Transient Analysis|Transient]]||[[#AC Analysis|AC Analysis]]||[[#DC Sweep|DC sweep]]||[[#Noise|Noise]]||[[#DC Transfer Function|DC Transfer]]||[[#DC Operating Point|DC op pnt]]<br />
|}<br />
{|table width="400" cellspacing="0" border="1" cellpadding="50" style="background-color: #DDDDDD" title="LTspice dialog box"<br />
|- align="center"<br />
| ''User options for the selected tab''<br />
|}<br />
__NOTOC__<br />
<br />
<br />
=== Transient Analysis ===<br />
Perform a Nonlinear Transient Analysis.<br />
<br />
This is a time domain analysis.&nbsp; Selected circuit signals may be displayed in the Waveform viewer as they are simulated, much like an oscilloscope on the bench.&nbsp; It basically computes what happens when the circuit is powered up and runs.&nbsp; Test signals are often applied as independent sources or may be taken from captured data stored on file.<br />
Syntax: .tran <Tstep> <Tstop> [Tstart [dTmax]] [modifiers]<br />
or .tran <Tstop> [modifiers]<br />
The first form is the traditional .tran SPICE command.&nbsp; Tstep is the plotting increment for the waveforms but is also used as an initial step-size guess.&nbsp; LTspice uses waveform compression, so this parameter is of little value and can be omitted or set to zero.&nbsp; Tstop is the duration of the simulation.&nbsp; Transient analyses always start at time equal to zero.&nbsp; However, if Tstart is specified, the waveform data between zero and Tstart is not saved.&nbsp; This is a means of managing the size of waveform files by allowing startup transients to be ignored.&nbsp; The final parameter dTmax, is the maximum time step to take while integrating the circuit equations.&nbsp; If Tstart or dTmax is specified, Tstep must be specified.<br />
<br />
Several ''modifiers'' can be placed on the .tran line.<br />
*'''UIC:&nbsp;''' Use Initial Conditions.&nbsp; Skip the D.C. operating solution and use user-specified initial conditions.&nbsp; Normally, a dc operating point analysis is performed before starting the transient analysis.&nbsp; This directive suppresses this initialization.&nbsp; The initial conditions of some circuit elements can be can be specified on a per-instance basis.&nbsp; <font color="green"><b title="UIC is not a particularly recommended feature of SPICE.&nbsp; Skipping the DC operating point analysis may often lead to a nonphysical initial condition.&nbsp; For example, consider a voltage source connected in parallel to a capacitance.&nbsp; The node voltage is taken as zero if not specified.&nbsp; Then, in the first time step, an infinite current is required to charge the capacitor.&nbsp; The simulator cannot find a short enough time step to make the current non-singular, and a 'time step too small convergence fail' message will be issued."> Extra Hint!</b></font><br />
*'''steady:&nbsp;''' Stop the simulation when steady state has been reached.<br />
*'''nodiscard:&nbsp;''' Don't delete the part of the transient simulation before steady state is reached.<br />
*'''startup:&nbsp;''' Solve the initial operating point with independent voltage and current sources turned off (but using any constraints specified by a .ic directive).&nbsp; Then start the transient analysis and linearly ramp on these sources during the first 20 us of the simulation.<br />
*'''step:&nbsp;''' Compute the step response of the circuit.<br />
<br />
<br />
=== AC Analysis ===<br />
Perform a small signal AC Analysis (linearized about the DC Operating Point).<br />
<br />
This is a frequency domain analysis whereby the ac small signal (i.e., linear) response of the circuit is calculated using complex variable arithmetic.&nbsp; First, LTspice finds the dc operating point of the circuit.&nbsp; Next, working about this operating point, LTspice calculates linearized small signal models for all nonlinear devices.&nbsp; Finally, using independent small signal ac voltage and current sources as the driving signal, LTspice solves the resultant linearized circuit in the frequency domain over the specified range of frequencies.&nbsp; <font color="green"><b title="By specifying just a single frequency point and sweeping (stepping) any circuit parameter instead, LTspice will display the ac response over that parameter's sweep range."> Extra Hint!</b></font><br />
<br />
This mode of analysis is useful for filters, networks, stability analyses, and noise considerations.<br />
Syntax: .ac <oct, dec, lin> <Nsteps> <StartFreq> <EndFreq><br />
The frequency is swept between frequencies StartFreq and EndFreq.&nbsp; The number of steps is defined with the keyword "oct", "dec", or "lin" and Nsteps according to the following table:<br />
<br />
{|table width="300" cellspacing="0" border="1"<br />
|- align="center"<br />
! Keyword || Nsteps<br />
|- align="center"<br />
| Oct || steps per octave<br />
|- align="center"<br />
| Dec || steps per decade<br />
|- align="center"<br />
| Lin || steps between <br /> StartFreq and EndFreq<br />
|}<br />
<br />
<br />
=== DC Sweep ===<br />
Perform a DC Source Sweep Analysis.<br />
<br />
This performs a DC analysis while sweeping the DC value of a source.&nbsp; It is useful for computing the DC transfer function of an amplifier or plotting the characteristic curves of a transistor for model verification.<br />
Syntax: .dc <srcnam> <Vstart> <Vstop> <Vincr> [<srcnam2> <Vstart2> <Vstop2> <Vincr2>]<br />
The <srcnam> is either an independent voltage or current source that is to be swept from <Vstart> to <Vstop> in <Vincr> step sizes.&nbsp; In the following example, the default BSIM3v3.2.4 characteristic curves are plotted:<br />
<br />
* Example .dc sweep<br />
*<br />
M1 2 1 0 0 nbsim<br />
Vgs 1 0 3.5<br />
Vds 2 0 3.5<br />
.dc Vds 3.5 0 -0.05 Vgs 0 3.5 0.5<br />
.model nbsim NMOS Level=8<br />
.save I(Vds)<br />
.end<br />
<br />
<br />
=== Noise ===<br />
Perform a Noise Analysis.<br />
<br />
This is a frequency domain analysis that computes the noise due to Johnson, shot and flicker noise.&nbsp; The output data is noise spectral density per unit square root bandwidth.<br />
Syntax: .noise V(<out>[,&lt;ref>]) <src> <oct, dec, lin> <Nsteps> <StartFreq> <EndFreq><br />
V(<out>[,&lt;ref>]) is the node at which the total output noise is calculated.&nbsp; It can be expressed as V(n1, n2) to represent the voltage between two nodes. <src> is the name of an independent source to which input noise is referred.&nbsp; <src> is the noiseless input signal.&nbsp; The parameters <oct, dec, lin>, <Nsteps>, <StartFreq>, and <EndFreq> define the frequency range of interest and resolution in the manner used in the .ac directive.<br />
<br />
Output data trace V(onoise) is the noise spectral voltage density referenced to the node(s) specified as the output in the above syntax.&nbsp; If the input signal is given as a voltage source, then data trace V(inoise) is the input-referred noise voltage density.&nbsp; If the input is specified as a current source, then the data trace inoise is the noise referred to the input current source signal.&nbsp; The noise contribution of each component can be plotted.&nbsp; These contributions are referenced to the output.&nbsp; You can reference them to the input by dividing by the data trace "gain".<br />
<br />
The waveform viewer can integrate noise over a bandwidth by ''ctrl-left mouse button'' clicking on the corresponding data trace label.<br />
<br />
<br />
=== DC Transfer Function ===<br />
Find the DC Small Signal Transfer Function.<br />
<br />
This is an analysis mode that finds the dc small signal transfer function of a node voltage or branch current due to small variations of an independent source.<br />
Syntax: .tf V(<node>[, &lt;ref>]) <source><br />
OR .tf I(<voltage source>) <source><br />
Examples:<br />
.tf V(out) Vin<br />
.tf V(5,3) Vin<br />
.tf I(Vload) Vin<br />
<br />
<br />
=== DC Operating Point ===<br />
Find the DC Operating Point<br />
<br />
Perform a dc operating point solution with capacitances open circuited and inductances short circuited.&nbsp; Usually a dc solution is performed as part of another analysis in order to find the operating point of the circuit.&nbsp; Use .op if you wish only this operating point to be found.&nbsp; The results will appear in a dialog box.&nbsp; After a .op simulation, when you point at a node or current the .op solution will appear on the status bar.<br />
Syntax: .op<br />
There is no guarantee that the operating point of a general nonlinear circuit can be found with successive linear approximations as is done in Newton-Raphson iteration.&nbsp; Should direct Newton iteration fail, LTspice tries a number of other methods to find an operating point.&nbsp; Below is a table of the methods used and the options settings required to disable a particular method.<br />
<br />
{|table width="300" cellspacing="0" border="1"<br />
|- align="center"<br />
! Method || Directive to Disable<br />
|- align="center"<br />
| Direct Newton Iteration || .opt NoOpIter<br />
|- align="center"<br />
| Adaptive Gmin Stepping || .opt GminSteps=0<br />
|- align="center"<br />
| Adaptive Source Stepping || .opt SrcSteps=0<br />
|- align="center"<br />
| Pseudo Transient || .opt pTranTau=0<br />
|}<br />
<br />
{{#widget:DISQUS<br />
|id=ltwiki<br />
|uniqid={{PAGENAME}}<br />
|url={{fullurl:{{PAGENAME}}}}<br />
}}</div>Rsfjr