Push-pull simulation

Discussion in 'The Projects Forum' started by renatomassa88, Jun 28, 2011.

  1. renatomassa88

    Thread Starter New Member

    Jun 12, 2011
    8
    0
    Hi, can anybody help with a push-pull simulation in LTSpice?
    Vin~300V
    Vout~15V
    Iout~1A
    Thanks
     
    • pp.png
      pp.png
      File size:
      32.1 KB
      Views:
      195
  2. StayatHomeElectronics

    Well-Known Member

    Sep 25, 2008
    864
    40
    What is the problem you are having?

    With transformers in LTSpice you usually need a reference point on the isolated side of the transformers, for calculation purposes. You can try connecting a ground on the output resistor R0 and see if the simulation runs. Sometimes a really large value of resistance can be added to help the simulation without affecting the results greatly.
     
  3. SgtWookie

    Expert

    Jul 17, 2007
    22,182
    1,728
    It will also help a great deal to add some parasitic values of resistance and capacitance to your transformer windings; otherwise the numbers get pretty unrealistic, and it will take forever to run. Even 0.1 Ohm series and 100pF parallel capacitance will work. Don't worry about the parallel resistance.

    Your R0 (load resistor) has a value of 1 Ohm. You'd need an output current of 15 Amperes to get 15v across it.

    I used a 1A current source as a load (right-click on a current source, click the "Advanced" button, fill in the desired current under DC, and under "Parasitic Properties" check the box below "This is an active load"). It's about as easy to use as a resistor, while providing just the amount of load that you specify.

    Since you don't have any method for voltage feedback, your output voltage will be a good bit more than 15v. You'd need to use a controller with a feedback path to get a regulated output.
     
    Last edited: Jun 29, 2011
  4. renatomassa88

    Thread Starter New Member

    Jun 12, 2011
    8
    0
    I put a ground reference on the load and changed it for a current source
    with 1A and with the "This is an active load" marked. I also included series
    resistance and parallel capacitance, but the output still keeps rising.
    Any sugestions?
    Thanks
     
  5. StayatHomeElectronics

    Well-Known Member

    Sep 25, 2008
    864
    40
    Can you give us a little more detail into the actual problem that you are seeing? Our responses to this point were answers to common problems seen in SPICE simulations.

    From SgtWookies response: "Since you don't have any method for voltage feedback, your output voltage will be a good bit more than 15v. You'd need to use a controller with a feedback path to get a regulated output."

    Is this the problem?
     
  6. renatomassa88

    Thread Starter New Member

    Jun 12, 2011
    8
    0
    I know that without a feedback the output won`t be perfect,
    but my problem is that the output keeps rising, no matter the
    duty cicle. The way I see, without a control, the output should
    be controlled by the duty cicle. I will do a charger with this
    circuit, but just to simulate I`ll do in an open loop.
    The signal in the mosfet`s are correct, but after the transformer
    the signal isn`t correct.
    Without the control the output can`t be nearly 15V?
    Thanks
     
  7. SgtWookie

    Expert

    Jul 17, 2007
    22,182
    1,728
    1) Reduce L5 to 18uH, and add parasitic series resistance of 10m.
    2) Increase the simulation run time to 1mS.
    3) Add a ground to the low side of C1.
    4) Re-run the simulation.

    You'll see the output voltage level off at ~29.2v.

    If you leave L5 at 470uH with no parasitic resistance, it will take perhaps 20mS for the output to settle back to around 29.2v; it'll peak somewhere around 45v due to the overshoot caused by the large value of inductance.
     
    Last edited: Jul 4, 2011
Loading...