Connect with us

Spice simulation

Discussion in 'Electronic Design' started by rickman, Dec 26, 2007.

Scroll to continue with content
  1. rickman

    rickman Guest

    I am using LTSpice III to simulate a filter using an LT1739 opamp.
    The filter is a two pole Multiple Feedback type set up for 4 kHz
    corner freq and a gain of 10. When I run the simulation it oscillates
    (in spite of the fact that the opamp is supposed to be stable at gains
    of 10 or more, but I guess the gain is not 10 at the higher freqs).
    So I have added a resistor and capacitor across the + and - input as
    indicated in the data sheet for the LT1739. That takes out the
    oscillation just fine. It appears that the cap value can be anything
    above about 2 pF to work and I will likely use 15 or 20 pF.

    When I use 4 kHz, 1 Vp to drive the input, it simulates ok. When I
    use 8 kHz, I get other oscillations. Playing with the component
    values I find I can stop these oscillations, but I still see a few
    perturbations. At a few time points, I see an abrupt spike in the
    output signal which then rings and damps out. I don't see any rhyme
    or reason to when these spikes occur and when it was oscillating, it
    would start at different times, as much as 80 mS into the

    What the heck is going on? The spikes don't seem to come from the
    input, an ideal sinusoidal voltage source. I only see the spike and
    oscillation in the output and feedback points. If I graph the output
    minus the inverting input to the opamp, it shows that the output is
    leading the input, so that seems to be the source. How can the opamp
    model produce this spikes and why would it be related to the input

    Should I be concerned about this in a real circuit? The original
    component values stopped the oscillations due to a lack of
    compensation. But I don't know if I need to worry about these "spike"
    related oscillations and the component values that stop them seem to
    be chaotic and not predictable. That makes me very concerned as any
    parasitics could easily make the "spike" oscillations reappear in a
    real circuit.
  2. John Larkin

    John Larkin Guest

    Try reducing the maximum time step in the simulation. Some of these
    things may not be real.

    You can make a parallel R-C oscillate if you set the sim parameters


  3. The minimum open loop gain should be at the order of G x Q^2. For the
    normal operation, you need about x10 more gain then minimum. Do you have
    that with LT1739?

    This could be a Spice issue. Try reducing the timestep.
    This could be a model issue. Try different opamp.
    You may run out of the open loop gain. Modify the circuit.
    However all of those problems may also indicate a general lack of
    stability of the circuit.

    Vladimir Vassilevsky
    DSP and Mixed Signal Design Consultant
  4. Guest

    Did you try using VCVS for opamp amps (i.e. finite gain but no BW
    limitations) in the circuit to insure the network is behaving as you

    It's a good idea to run the filter with VCVS and the macromodels of
    the opamp just to see the Q-enhancement effects.

    Make sure you use all 4 parameters on the .tran line. The tmax
    parameter is the important one.
  5. Jim Thompson

    Jim Thompson Guest

    Many active filters, which have even moderately high "Q", will clip
    internally and do all kinds of weirdness at certain signal levels.

    ...Jim Thompson
  6. Guest

    From the description, this sounds like a one amp two pole filter. The
    "internal clipping" you mentioned is a dynamic range adjustment issue.
    This isn't always included in text books for some reason. Basically,
    you sweep the filter, finding the peaks of every op amp node. Then you
    scale each node in a manner where you only adjust the gain, not the
    time constants. If you do this, the noise is minimized and nothing
    should clip internally.

    The proper frame of mind is to think of every op amp output is a
    filter output, even if only one op amp output has the desired
  7. rickman

    rickman Guest

    Thanks to everyone for their comments. I never found out why the
    simulation has the spikes in the filter output, but I have to assume
    that is an artifact of the simulation. I did finally get a handle on
    the compensation required and have a circuit working well in
    simulation. We will see what happens when I construct it, but I am
    confident that it will work as expected.
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