RLC Circuit with unusual parameters values

Discussion in 'Homework Help' started by Mirko Hu, Apr 30, 2016.

  1. Mirko Hu

    Thread Starter New Member

    Nov 19, 2015
    3
    0
    Dear all,

    I have a problem performing the transient analysis of my RLC circuit on LTSpice.

    Portraing the analysis of the circuit (calculating the transfer function etc.), with a gain of 32 on VDVC, I should obtain a slightly damped oscillation (therefore a stable oscillating system).

    Though, the transient analysis shows me random traces (for both the V's and I's) that look like noise. I guess the problem lays on the values of the inductances that are incredibly high (but correct in my case). Are there any settings in LTSpice I could modify to deal with this situation?

    Thanks everyone.
     
  2. MrAl

    Well-Known Member

    Jun 17, 2014
    2,431
    490
    Hi,

    It looks like you dont have ANY energy going into the system at all. That means it will be operating on the parasitic behavior of the spice models and simulator analysis technique, which challenges the models and simulator too much.

    In any circuit you have to input at least a little energy to get it going, like with an oscillator circuit that never oscillates until a little energy is injected. In real life it would start, but in simulation it wont start.

    Try using some extra source or give one of the caps some initial energy to get it going.
     
  3. Mirko Hu

    Thread Starter New Member

    Nov 19, 2015
    3
    0
    Hi MrAl,

    Thank you for your reply. I have tried two different schematics namely by adding a source (with a pulse) on a line and by setting an initial condition on a capacitor, but both methods fail to return the behaviour I am expecting...
    I have attached the plot of the simulation with IC. The simulation speed is very low and the values seem to be random.
    Have you any other ideas?
     
  4. MrAl

    Well-Known Member

    Jun 17, 2014
    2,431
    490
    Hello again,

    First, where did this circuit come from, is it an oscillator, and is it known to be stable?
    Also, what behavior are you actually expecting to see?

    From the simulation results it looks like the numerical method being used is saturating. That probably means the differential equations required to describe the circuit are too stiff or the circuit is unstable. The numerical methods all rely on calculated numerical derivatives, and the derivatives all depend on differences, and if the differences get too small then the truncation due to limited precision causes it to go to zero for one calculation, then non zero for another, then back to zero, etc., which looks like an oscillation even when there is really no oscillation there, at least not on purpose.
    The best method to try using though is Gears in these simulators, followed by modified trapezoidal, then trapezoidal.

    If there's no way to get it to work in a simulator, then you'd have to try to solve it yourself using your own program and write up the equations needed. Since the order is so high it's doubtful that an analytic solution is viable, so a numerical solution is probably the only way. This would involve writing a set of equations for the circuit, writing your own numerical differential equation solver, and because of the stiff problem you might have to use a higher precision number cruncher algorithm also. Most computers are limited to 16 or 17 digits natively, but you can go higher with software. The drawback is the algorithm takes longer to run. Some simulations will take longer than others due to the complexity of the equations in any simulator or number cruncher.

    You might find algorithms that solve differential equations on the web. Algorithms like the Runge Kutta-Fehlberg 45 or the Runge Kutta 78 for example. You might also find higher precision numerical number crunchers on the web too. Anything higher than order 7 or 8 will most likely also require a higher precision number cruncher too.

    You could try various other things too in the simulator, maybe we are just overlooking something.
    Some things that will matter are:
    1. Some initial energy injection is required.
    2. Do not solve for initial operating point.
    3. Use a small time max time step, but try to vary it. Sometimes one step value works better than another even if it is larger.
    4. Try ramping up power supply sources.

    To get the equations to be a little less stiff, you could try placing some resistances in series with caps or inductors, but yes that will change the circuit a little. I dont know where this circuit came from so i dont know what kind of changes would be considered acceptable. For example, real caps usually have some ESR anyway.

    Another idea is to try to get the circuit to work with any values, then start to move those values back to the original values and see when it starts to fail. That might tell you something.

    There is also frequency scaling, where the component values are all changed, a simulation run on the scaled circuit, then the results are scaled back to what they would be with the real values. This works well in AC circuits, but i'd have to look some things up myself to see how it works in transient circuits again. If the circuit ends up too stiff again however we might end up with the same problem anyway ;-)
     
    Last edited: May 1, 2016
  5. Mirko Hu

    Thread Starter New Member

    Nov 19, 2015
    3
    0
    Hi MrAl,

    Thank you again for your support and your long reply.

    I am using analogies between the fluid/thermal domain and the electrical one to build the circuit model of an oscillating thermo-fluidic device, i.e. a device where there is a fluid that oscillates thanks to some thermal energy.

    I have such big values for the resistances and inductances because they represent respectively the resistance to the movement of the fluid in the oscillator (e.g. a valve) and the fluid inertia.

    I have calculated the transfer function with MATLAB and performed a stability analysis using the root locus. With a gain value smaller than 32.2, I should have a stable system.

    I would like to use LTSpice because it is good to observe the behaviour of voltage and current, I wonder if there is any way to 'rescale' the circuit in order to obtain an equivalent circuit...

    Anyway I am going to try your suggestions.

    Thanks again :).
     
  6. MrAl

    Well-Known Member

    Jun 17, 2014
    2,431
    490
    Hello again,

    Ok then a quick note: determine where the initial heat gets into the construction and create a voltage or current source to model that input, and apply it to wherever it appears in the physical structure. That is missing from the diagram you showed so far and that could make a difference because that will be the primary drive of the structure. Without that it would be almost like creating a power supply without any power source input :)

    So far we tried using an initial condition generator, but that may not be needed if the drive source is present, and there is always some thermal input coming from somewhere. If there are initial temperatures in some areas though then initial condition generators might still be needed, one for each mass for example.

    When i first saw it i thought it was some sort of oscillator because there were no input sources :) Now it is starting to sound almost like a heat pipe heat sink.

    Another small note, using a gain so close to the crossover unstable gain value could result in a simulation that takes a long time to complete or takes long just to compute some time steps. Backing down a little bit more would probably speed up the simulation, just to get some initial results a little faster.
     
Loading...