Problem with Simulating Flyback Converter

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?

I see following issues here:
For driving MOSFET, you should not use Digital stimulus. it may not be able to switch the MOS properly. Instead use VPULSE and select appropriate voltage level.
I am not able to understand the Transformer secondary side connection? Why are you connecting that to MOS Drain, I believe Transformer secondary should be connected to ground.
What duty cycle you are trying to select ? The screen capture you attached it appears to be 50%, so that won't give you any step up effect due to topology. You should use >50% to get the boost effect.
Check the primary current, you have not mentioned the switching frequency. You should not get excessive voltage drop in R2.

Hope these helps you get desired result.

Actually I have simulated the circuit with vpulse and get the same result. I have chosen 10KHZ for the switching frequency.
The schematic is not a normal flyback, however when I ground the second winding voltage drops to 45V (In comparison with the 90v when it's not grounded). I have the same result regardless of changes I make to my circuit. I don't know where the error is?

Since a Flyback transformer is a coupled inductor you might have better results simulating with an inductor for the primary and put an ideal transformer element with desired turns ratio across inductor.

You will need some load on the output otherwise voltage will keep rising. If you are getting limited to 90 vdc it may be the breakdown voltage on the diode model used.

So what you have in your schematic is a tapped inductor boost converter, not really a flyback (though they are similar).

Anyways, you say you have 10KHz as your frequency, but in your spice schematic it shows your digital source with on/off times of 10ms...

Also make sure you are driving the gate with enough voltage. Like between 10-15 volts. You should verify that when the gate voltage is high, the drain voltage is very near 0V.

Also, as stated above, if that transformer you have in your schematic is an ideal model, then it definitely won't work as expected. Either give it some realistic parameters (if you can) or put some additional magnetizing inductance on its primary or secondary.

I don't know, if your 1N914 model has a breakdown voltage. A real 1N914 won't work for 200V. You also didn't mention the coupling factor set for the transformer. With K=1, the two inductors behave like an ideal transformer. A real tranformer would have e.g. K=0.9 to 0.95.

Of course, the PSPICE simulation can tell you exactly, why the output voltage doesn't goes above 90 V. You just need to get familiar with the Probe tool, and have a basic understanding of the circuit operation.

Edaboard members can more easily check your results, if you post a zip archive of the PSPICE design.

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.

As suspected, the unsuitable rectifier diode turns out to be the main reason for the output voltage limitation. You can e.g. place a 300 V type BAW101.