Flyback converter Problem

Discussion in 'The Projects Forum' started by mashmohsen, Aug 22, 2011.

  1. mashmohsen

    Thread Starter New Member

    Aug 4, 2011
    7
    0
    Hi all

    I am a newbie in power electronic field. I have a flyback converter which I cannot get the desired result from the simulation in Pspice. I am not sure if the problem is from the transformer or the switching.
    The circuit is supposed to convert a 3.7 VDC from a Battery to 200 VDC.
    I am using the following parameters for the circuit:
    Cin=4.2uF
    Chv=0.22uF
    The Transformer Parameters would be as followed:
    L1=6.2uH
    R1=1 Ohm
    L2=300uH
    R2=42.7Ohm (R1 and R2 are supposed to be the winding resistance)
    right now I get 90 VDC regardless of whatever change I make I my circuit (changing the turn ratio, changing the input voltage)
    I have tried to simulate it in MatLab simulink and I get the same result.

    Could you please help me figure out where the problem is and why I cannot get the 200VDC output?

    [​IMG][​IMG]
     
  2. SgtWookie

    Expert

    Jul 17, 2007
    22,182
    1,728
    Find the datasheets for the MOSFET and diode that you are using.

    Make certain that they are rated for the voltage and current that you expect to see in the circuit.
     
  3. ifixit

    Distinguished Member

    Nov 20, 2008
    638
    108
    An ON time of 20uS, an OFF time of 10uS, and a resistive load of 40K equals a Vhv of 200V. I changed the diode to a UPS600 which has a PIV of 600V.
     
  4. DickCappels

    Moderator

    Aug 21, 2008
    2,651
    632
    But read that schematic again...the on and off times are in milliseconds -that's a lot of amps on the drain! (I have not used P-Spice, but I assume that ms means milliseconds). You need to make your on and off times microseconds, not milliseconds.

    Have a look at the drain current and voltage waveforms in the primary, and if possible, please post them.
     
  5. SgtWookie

    Expert

    Jul 17, 2007
    22,182
    1,728
    ifixit,
    there's a problem with using the UPSC600 model in LTSpice; those SiC diodes have virtually zero recovery time, but MicroSemi has no documentation available that they ever made a diode of that part number.

    Even fast-recovery or ultrafast diodes have a far greater recovery time than that SiC model. I recently tried using some models for ultrafast diodes to compare with the UPSC600 model; the results weren't encouraging at all - the recovery time added a lot of inefficiency to the simulation, but it's probably a lot closer to reality.

    As I see it, the problems our OP is having with their simulation are:

    1) The Vdss rating of the IRF150 is only 100v. At that point, the intrinsic body diode breaks down, and clamps the output.

    2) The PIV of the 1N914 will be somewhere between 75v and 100v, depending on who designed the model. Above that, and it'll act like a clamp in the simulation.

    3) Although it won't impact the simulation much, the forward current limitations of the 1N914 would likely vaporize the junction during start-up in a real-world trial.

    4) The modeling of the winding resistance is poor. It would be much better if the windings were split, and the resistance placed in between the windings. It would be better yet if they could specify the winding resistance directly for the windings; but I don't know if their simulator has that provision available.
     
  6. SgtWookie

    Expert

    Jul 17, 2007
    22,182
    1,728
    Yes, the on/off times for the MOSFET are a big problem, too. The inductors would have to be a great deal larger to get the current to a manageable level.
     
  7. ifixit

    Distinguished Member

    Nov 20, 2008
    638
    108
    Hi Sgtwookie,

    I like the circuit, it works well as a concept, but does need a better diode than a 1n914. LTspice doesn't have a schottky model with a 200V PIV:(. The mosfet Vd max only needs to be 50V or so because it doesn't "see" the higher voltage at the output at Vp.

    It is just a simulation and my purpose was to show the OP how it can be made to work in simulation with minimal changes to the components. Making the circuit more eff will be a bigger challenge.

    Hi Dick,
    Sim file is attached, I upped the frequency to make it more efficient.
     
  8. mashmohsen

    Thread Starter New Member

    Aug 4, 2011
    7
    0
    Actually I know that the problem is because of my element choice, so I simulated the circuit in matlab simulink and the same problem occurs. i will attach both matlab and pspice model.
    thanks guys for your help.
     
  9. rajeevranjan1189

    New Member

    Oct 16, 2014
    2
    0
    [​IMG][/QUOTE]
     
  10. rajeevranjan1189

    New Member

    Oct 16, 2014
    2
    0
    Whatever transformer you have used that will not work like flyback transformer in pspice. Try PSIM or some other software otherwise use couple inductor in Pspice that might be helpful for you. Flyback transformer behave more like inductors. Just try with couple inductor and update me with results.
    Regards
    Rajeev
    +919972725500
     
  11. alfacliff

    Well-Known Member

    Dec 13, 2013
    2,449
    428
    a 1n914 diode isnt rated for enough voltage, only 100 volts.
     
Loading...