380V to 18V buck converter, troubles simulating

[crutschow]

If you are getting 12Vpp centered around 0 then it sounds like you have the oscilloscope AC coupled. The circuit, by itself can't generate voltages below 0V.

 

[Unsureofwhattodo]

You were correct about the AC coupled oscilloscope. I'm embarrassed to have forgotten about that.

 

[Unsureofwhattodo]

So I'm focusing my efforts on at least getting a PSPICE design for a 380-18V buck converter using the bootstrap driver you initially suggested (which after looking at I like a lot). I figure if I can't physically produce a 32-16 despite having a working simulation, I can at least try to provide as much as I can when I turn in my project.

So I've been trying to design the compensation components for the error amplifier, and I've been following the equations on page 5-14 of the paper you provided earlier. My variables were:

Fs= 10kHz
Vp= 3V (I wasn't entirely sure what this voltage is, is it the max voltage of the sawtooth in the PWM chip?)
L=1650 uH (both L and C were taken from DayCounter Inc's website from their calculator)
C= 12uF
Vi= 380v (I didn't know what other Vi it could be)

As I moved through the calculations, the only value I was really concerned about was R2 = 60 ohm. Here are all the values I got for the set up:

R1 = 10k
C1= 15nF
R2 = 60
C2 = 25uF
C3 = 80pF (I found a suitable 12uF cap with a 40mOhm ESR)

So I suppose the question is: Is it acceptable/expected to have a K of 1/166? If not, what should I do differently? Thanks for the continued help over this whole weekend. I greatly appreciate it.

 

[Unsureofwhattodo]

So I couldn't get the whole thing to run in PSPICE, so I took a step back and just tried to get an ideal version of the bootstrap driver and the buck converter together working.




This is what I have so far. Am I just misunderstanding how to set up the driver?

 

[crutschow]

Offhand the circuit looks ok. Do you think it's not working?

The voltage being too high is likely the result of switching delays which makes the duty-cycle larger than ideal.

 

[Unsureofwhattodo]

I'm concerned about why I am getting around 40V at the output? I'm trying to get 18V.

 

[crutschow]

I was editing my post while you were replying. Look at the output waveform at the inductor input.

 

[Unsureofwhattodo]

This is the input at the inductor



It seems to be 380 like it's supposed to.

Seems my TR/TF was effecting the output voltage. Which I can assume was messing with my DC when it's already so low?

 

[crutschow]

Expand the time frame so you can see the duty-cycle of the waveform at the inductor and compare it with the signal waveform. They are likely different due to circuit delays.

 

[Unsureofwhattodo]

It seems so. Can you take a look at one of my earlier posts about the calculations for the compensation values? With this simulation I can say show that this circuit will work provided I can give it the proper signal, which is easy enough to do. The only issue is making sure I have those compensation values correct. If I have those I have a whole circuit that I have confidence in working when we can order one of the drivers. Thanks in advance!

 

[crutschow]

I didn't crank through your calculations but your approach seems correct. Vi is indeed the 380V input and Vp is the PP value of the sawtooth.

I designed a buck regulator some years ago and initially simulated the control loop with a linear simulation to optimize the compensation values. For that you just substitute a linear gain block for the PWM modulator. The gain of this block is basically Vi divided by Vp (since a 3V input change causes the PWM duty-cycle to change from 0% to 100% and the output voltage from 0V to Vi). Thus, in your case, it would be 380V / 3V = 126. So you put an AV=126 gain block in series with the compensation op amp driving the output inductor and capacitor. AC simulation of that to get a Bode plot will give a good indication of whether your loop with the actual PWM circuit will also be stable.

If you close the loop by connecting the capacitor output to the op amp input, you can do a transient simulation to look at the loop transient response and any overshoot or ringing in the loop, which is also a good indication of loop stability.

The linear simulation I did gave stability values very close to those obtained with the actual circuit.