Connect with us

Need help with simulation

Discussion in 'Electronic Basics' started by bench, May 8, 2004.

Scroll to continue with content
  1. bench

    bench Guest

    Hi everyone,

    I am having trouble simulating an astable multivibrator and
    I was wondering if anyone can help me. I am using
    a package called Circuit Maker 6 and the circuit has
    already been inputted and all you need to do is download
    the file
    ; rename it without the .txt extension (as it is a .ckt file) and
    see if you can get it to oscillate. I am not sure what is wrong
    with the circuit, maybee the resistors or capacitors have been
    assigned wrong values. I initially used generic npn transistors,
    but then I tried the 2n2222, but nothing seems to help.
  2. You need to add a .IC (Initial Conditions) device/command to at least
    one of the capacitors, to get oscillation started. I've shown it here,
    using your otherwise unchanged circuit:
  3. CM6 has an example circuit which is almost exactly the circuit you
    posted... Look for 'Astable.ckt' amongst the examples.

    With regards to your circuit, your timing values are pretty big. If
    the oscillator worked with your values, it would oscillate at about
    3.5Hz, which would be much too slow to see with the simulation values
    you have set. Also, you may need initial conditions for some of the
    nodes to get the oscillation going in the first place. I got your
    circuit going by changing the cap values to C1=500pF and C2=1nF,
    R2=R3=47k, and putting initial conditions on the collectors of the
    transistors as 0V (on the left) and 9V (on the right). Also, go to the
    transient setup, and change the stop time to 500us, and the step time
    and max step to 1us.

    Here follows far more information than you possibly want to hear about
    the oscillator.

    The oscillation frequency is near -ln(.5) * (R1*C1 + R2*C2). Thats
    because the fall in the collector on one side (when the transitor
    turns on) drags the base of the other side down 9V through the
    capacitor, so it has to increase back to 0.7 to turn on again. It does
    this by charging through the cap/resistor pair. The equation governing
    the time of recharge of a cap C through a resistor R can be shown to

    Vx -Vs = (Vt - Vs) exp(-t/RC)

    Where Vs is the starting voltage, Vx is the 'target' voltage, Vt is
    the voltage at the other side of the resistor, t is the time required,
    and R and C are of course the values for those components. Since the
    voltage is dragged down from 0.7 to -8.3, and has to climb back up to
    0.7 again to turn on the transistor and complete that part of the
    cycle, you have

    Vs = -8.3V
    Vx - Vs = 0.7 - (-8.3) = 9
    Vt - Vs = 9 - (-8.3) = 17.3V
    C1 = 500pF, R2 = 47k
    C2 = 1nF, R3 = 47k

    So (solving the above for t, and noting that there are two RC
    oscillators going, one after the other...)

    t = -ln(9/17.3) * (500pF * 47k + 1nF * 47k)
    = 0.653 * (70.5u)
    = 46u

    Therefore, the frequency of the oscillator with the values given above

    f = 1/46u = 21kHz

    This matches pretty well with the simulated value, which is around
    20kHz. It doesn't match exactly, because the Vs above isn't
    really -8.3; its something a bit less negative, because of various
    effects, so it doesn't go down 9V, more like 7.5V... We could take
    that into account, but these values are close enough, given that the
    caps and resistors you'll use are probably 5% to 10% tolerance.

    By the equations above, its easy to see that you can control the 'duty
    cycle' of the oscillator by simply changing cap or resistor values. By
    keeping the sum constant, the frequency will be kept constant.

    Bob Monsen
  4. You beat me, Terry... Actually, I found that it oscillates without the
    initial condition. I guess circuitmaker is putting in some randomness
    to get things started.

    The OPs problem was the time scale of his simulation. The default of
    5us won't show much change. However, if you scope the collectors of
    both transistors, you see divergence almost immediately.

    One thing I found really interesting was zooming in on the startup of
    this circuit. If you set the transient parameters to a stop time of
    10ms, and scope the collectors, you see the startup quite clearly.

    Bob Monsen
  5. I should have added that, although the circuit I used was unchanged, I
    too immediately changed the time scale from the default to 1 s, as you
    see from the screenshot.

    That also roughly shows the interesting startup effect you mentioned.
  6. bench

    bench Guest

    My waveform is for some reason a bit erratic comapared
    to your results, here is my snapshot.
    I took a 10 seconds range because the waveform seems to
    change and 10 seconds are required to see this.
    My simulation step is 20mS and max
    step is 200mS (not sure what this max value is for).
    B.t.w. thanks for all the formulas, I shall have
    a look at them after I can sort this issue first.
  7. 50ms is much too big. Doing this kind of numerical integration is
    approximate, and so errors creep in after a bit. In a real system,
    this won't happen.

    If you decrease the timestep and max to 100u/100u, you will get better

    Bob Monsen
  8. That's the reason for your strange results. Nothing changes much after
    about 50 ms. That's why I used a Stop Time of 1 s. Certainly no need
    for 10 s! And my choice for Step and Max. Step of 1 ms wasn't
    From CM6 Help (which I suggest you study):
    "Step Time is the suggested computing increment, but the timestep will
    be varied automatically by XSpice in order to properly converge. Max.
    Step limits the varying size of the timestep that XSpice can use when
    calculating the transient data; by default, the program chooses either
    Step Time or (Stop Time - Start Time)/50, whichever is smaller.
    Typically, Step Time and Max. Step would be the same value."

    Robert: Following your post, I too subsequently re-ran it OK *without*
    the .IC command. Not entirely sure why that didn't appear to work
    first time I tried. May have been my carelessness. But I do recall
    oscillators like this needing an initial condition. 555 astables seem
    particularly fussy!
  9. If you look at the sample (Astable.ckt) it has a note describing the
    usage of .IC. It even works when everything is equal (like in the OP's
    circuit.) I've had this kind of thing fail in other spices before, but
    circuitmaker seems to be ok with it. They appear to factor in some
    thermal noise which gets things going properly.

  10. bench

    bench Guest

    Thanks to all !!!!!!!
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