How to simulate the RC relaxation oscillator using LTspice

Discussion in 'General Electronics Chat' started by jLuca, May 8, 2015.

  1. jLuca

    Thread Starter New Member

    May 8, 2015
    2
    0
    Hello everyone, how can I simulate the circuit I attached (RC relaxation oscillator) using LTspice? The problem arises when I simulate it with the .tran directive, the output (V2) is a costant value (different from +/- supply voltages). I tried to use the .ic directives to set an initial condition (V of the condensator = 0 and V2 = 0) but it didn't help (the simulation is different from the previous case but it's not what I expect from the theory: the V2 voltage value drops from the supply voltage value to zero and then stays zero; furthermore, the time it takes to decrease is different from the time constant of the RC circuit).
    Tomorrow I will also link the LTspice circuit and simulations (I don't have them right now).
    Last note: I choosed randomly the op amp (LT1001).
     
  2. MikeML

    AAC Fanatic!

    Oct 2, 2009
    5,450
    1,066
    The circuit is incorrect. It cannot oscillate. See, LTSpice is telling you something.
     
  3. RichardO

    Well-Known Member

    May 4, 2013
    1,230
    382
    And, why not???
     
  4. crutschow

    Expert

    Mar 14, 2008
    13,000
    3,229
    The circuit simulates fine in LTspice with R1 = 10kΩ and C = 0.1μf.
    What R1C values did you use?
    Try using the options Skip initial operating point or Start DC supplies at 0V.
     
  5. MikeML

    AAC Fanatic!

    Oct 2, 2009
    5,450
    1,066
    Well actually, it can, but there is a problem with the LT1001 model. Here it is with a LT1013. Note that to make it start quickly, I use the .IC V(v1)=-1n to get it started.

    63a.gif

    Here it is repeated with without the .IC directive. Note that it finally does start on its own if the simulation run time is increased. There is always some numeric "noise" in the solver that eventually gets amplified by the open-loop gain of the opamp to the point that it takes off.

    63b.gif

    Here it the aberrant behavior with the LT1001. Note the input current to the non inverting input pin. That is non-physical. This initially (with the values I had) prevented it from oscillating.

    63c.gif
     
    Last edited: May 8, 2015
  6. jLuca

    Thread Starter New Member

    May 8, 2015
    2
    0
    I did another test using another computer (see picture attached), now the circuit is being simulated quite correctly. Maybe there is some problem with the LTspice installed on the other computer. I also tried to use the LT1013 and it works better than LT1001.
    Thanks for your help.
     
Loading...