Connect with us

The limits of .ac analysis in LTSpice

Discussion in 'CAD' started by Paul Burridge, Jan 8, 2004.

Scroll to continue with content
  1. Would I be right in thinking that it's a waste of time trying to do a
    frequency response sweep of something like a power amplifier with the
    AC analysis? If any of the circuit elements need to be explored under
    non-linear conditions when 'tuning for maximum smoke' as they say,
    then is this beyond any current flavour of Spice?


  2. mikem

    mikem Guest

    I would just use Transient Analysis with sinosoidal inputs turned up to
    levels where distortion might become an issue. You can use an FFT to
    post-process the output waveforms to evaluate them for

    See the attached example:

    paste the following to a file called LargeSignal.asc, and open it
    with LTSpice



    Version 4
    SHEET 1 880 680
    WIRE 80 224 -32 224
    WIRE -32 224 -32 240
    WIRE -32 320 -32 352
    WIRE -32 352 128 352
    WIRE 128 352 128 240
    WIRE 128 144 128 128
    WIRE 128 32 128 0
    WIRE 128 0 272 0
    WIRE 272 0 272 176
    WIRE 272 352 272 256
    WIRE 272 352 128 352
    WIRE 128 384 128 352
    WIRE 128 128 336 128
    WIRE 128 128 128 112
    FLAG 128 384 0
    FLAG 336 128 out
    SYMBOL nmos 80 144 R0
    SYMATTR InstName M1
    SYMATTR Value IRF7201
    SYMBOL res 112 16 R0
    SYMATTR InstName R1
    SYMATTR Value 10
    SYMBOL voltage -32 224 R0
    WINDOW 123 0 0 Left 0
    WINDOW 39 0 0 Left 0
    SYMATTR InstName V1
    SYMATTR Value SINE(2.9 0.1 1000)
    SYMBOL Misc\\battery 272 160 R0
    WINDOW 123 0 0 Left 0
    WINDOW 39 0 0 Left 0
    SYMATTR InstName V2
    SYMATTR Value 12
    TEXT -16 384 Left 0 !.tran 5m
  3. analog

    analog Guest

    No, it's may only be a waste of time if you don't know what you are
    doing and are unaware of the effect of operating point on small signal
    As with any linear circuit, for a power amplifier an ac analysis
    would most likely be used to check loop gain and closed loop frequency
    response. The only difference with a power amp being that one would
    probably want to check response at several dynamic operating points,
    not just at quiescence. A poorly designed amplifier may break into
    "small-signal" oscillations only with certain loads when driven hard.

    What an ac analysis won't do is tell you anything about non-linear
    large signal behavior such as recovery from being driven into
    saturation. Both ac and transient analyses are indispensable design
    tools. -- analog

    Download the full featured *free* LTspice circuit simulator at:

    "The small-signal(linear) AC portion of LTspice computes the AC com-
    plex node voltages as a function of frequency. First, the DC operating
    point of the circuit is found. Next, linearized small-signal models
    for all of the nonlinear devices in the circuit are found for this op-
    erating point. Finally, using independent voltage and current sources
    as the driving signal, the resultant linearized circuit is solved in
    the frequency domain over the specified range of frequencies."

    -- the LTspice help file on Dot Commands (.ac)
  4. Russell Shaw

    Russell Shaw Guest

    For something like a class-C RF amp, it would be useless. However, it
    would give an idea of the input-output isolation capability of small
    signals when the amp is not being driven.
  5. No.

    Its very useful, but does not contain the full story. In addition the
    small signal ac distortion capability of spice gives can give a
    reasonable quick guide of distortion over a range of frequencies.
    Dont understand what you are saying here. Non-linear/large signal
    conditions are handled in spice by a transient run. One can then use
    this data to do an FFT to obtain a spot frequency measuring of

    Kevin Aylward
    SuperSpice, a very affordable Mixed-Mode
    Windows Simulator with Schematic Capture,
    Waveform Display, FFT's and Filter Design.

    That which is mostly observed, is that which replicates the most.
  6. Rick

    Rick Guest

    Makes you wonder why Berkeley never implemented Harmonic Balance in SPICE ;-)
  7. Not really. They were mostly students, so no doubt they were down the
    pub, attempting to pick up women.

    Kevin Aylward
    SuperSpice, a very affordable Mixed-Mode
    Windows Simulator with Schematic Capture,
    Waveform Display, FFT's and Filter Design.

    "That which is mostly observed, is that which replicates the most".

    "quotes with no meaning, are meaningless" - Kevin Aylward.
  8. broken

    broken Guest

    Spice Girls, obviously.
  9. How (in simple terms) do harmonic-based simulators function which
    makes them better than spice for RF stuff?
  10. Thanks, Mike, I ran your example and it nicely illustrates clipping
    and gate threshold biasing, but I'm quite happy with TA; have no
    insurmountable problem with it and it's info on the correct use of
    *.AC* that I need to acquire.. Perhaps I haven't expressed myself
    adequately. it has been known. :) I
    I've read the technical explanation of what it does as provided in the
    LT spice help file but... I try to rephrase it.
  11. Steve Hamm

    Steve Hamm Guest

    That was a matter of timing, I think. Berkeley had Tom Quarles
    working on doing SPICE3 about the same time Ken Kundert was working on
    the original (Berkeley) Spectre. I think Ken didn't want SPICE's
    baggage, and there was a bit of rivalry there. But that was before
    the Krylov methods had been turned into a tool for beating down the
    harmonic balance problem. But there are a few industrial circuit
    simulators that have, basically, SPICE + harmonic balance.
    Harmonic balance solves Kirchoff's equations in the frequency domain,
    for as many harmonics as you can afford. The models used are the
    standard nonlinear models like those used for transient analysis; AC
    analysis linearizes about a single operating point. The result is a
    spectrum of the circuit at steady-state, taking into account all the
    effects one expects to see from the nonlinearities, similar to what
    one would get from FFT'ing the 'final' period of a transient analysis.
    Except: multiple nonrelated tones can be used, and for this type of
    simulation the appropriate transient analysis could be measured in
    geological time. The steady-state spectrum can be considered as a
    time-varying operating point for further analysis, such as periodic
    noise analysis.

    Anyway, most of the standard measures of RF circuit 'goodness' are in
    the frequency domain and are best done in harmonic balance: IP3, IM
    calculations, etc. are done most easily as sweeps or sequences of
    harmonic balance simulations.
  12. So the upshot being that whereas a real world RF circuit might throw
    out all sorts of spurii, a Spice simulation of it would only show one,
    principal signal; the HB method shows all the crap as well; like you'd
    see of the real circuit had you used an oscilloscope of suitably high
    bandwidth to view it? Is that a consequence of what you're saying?
  13. Russell Shaw

    Russell Shaw Guest

    No. Spice will generate the same IMD from multi-tones, but the lower
    level products are easily lost in numerical noise, and are a pain to
    extract with FFT.
    HB is best for time-varying circuits with one principle
    large signal and any number of smaller signals.
  14. Best why? Is it simply _faster_ or is it more revealing in some way?
  15. Russell Shaw

    Russell Shaw Guest

    More dynamic range. Small signals aren't lost in noise.
  16. Steve Hamm

    Steve Hamm Guest

    Actually, the numerical noise point is good. The error mechanism in
    harmonic balance is mostly through having too few harmonics. The
    differential equations are solved in the frequency domain, where d/dt
    becomes multiplication by Laplace 's' -- no difference approximation
    error as in transient analysis. And harmonic balance is a uniform
    approximation method, unlike transient analysis which can accumulate
    error with each timepoint. For circuits where the waveforms are
    represented well by a reasonable number of harmonics, accuracy is good
    and the noise floor is orders of magnitude lower than transient
    analysis. So, as you say, small mixing products are less likely to
    get lost in the numerical noise.
    Hmmm. This is true for the periodic steady-state methods, which can't
    easily handle multiple large signals -- to be efficient, they really
    want one large signal, then they approximate the small signals as
    perturbations on a time-varying operating point. But multi-tone
    harmonic balance can handle multiple large signals -- wouldn't be very
    useful in RF if it couldn't. And the frequencies of these signals
    need not be related. This is a killer for time-domain methods, since
    the period required must be one for which all signals are periodic,
    which could be _very_ long. In this case, harmonic balance can be
    _much_ faster than transient analysis.

    Transient analysis and periodic steady-state methods have an advantage
    in that they don't care (much) about how horribly nonlinear the
    circuit is. Harmonic balance does care, in that more harmonics are
    required to (a) get convergence, and (b) represent the waveforms well.
    And more harmonics will slow the HB simulation. So there are
    certainly appropriate places to apply both...
  17. Russell Shaw

    Russell Shaw Guest

    That's what i meant, but worded it wrong. Multiple large signals
    can be handled, but if that's all you need, then spice can do it.
Ask a Question
Want to reply to this thread or ask your own question?
You'll need to choose a username for the site, which only take a couple of moments (here). After that, you can post your question and our members will help you out.
Electronics Point Logo
Continue to site
Quote of the day