0:01

In this lecture,

we discuss design verification using average circuit simulations,

in particular we would like to focus on closed loop POL voltage regulation.

As an example, let's look at the switching circuit model of the Synchronous Buck POL

voltage regulator designed earlier in this specialization.

0:43

processed by the error amplifier,

which produces the control voltage at the input of the pulse width modulator.

In response to the control voltage, the pulse width modulator produces

pulsating waveform c, width duty cycle that ultimately controls the

conversion ratio of the converter.

That control signal passes through a dead-time circuit and

the gate drivers to control the two power MOSFETs.

So we will first do a transient simulation of this circuit.

1:49

So here is the result of that transient simulation of the switching circuit model.

The output voltage is ramping up.

Finally reaching it's steady state value equal to the reference, 1.8 volts.

In response to a step load transient here, which occurs at 150 microseconds.

We have a slight dip in the voltage and a very quick recovery,

this is a fairly fast voltage regulator.

And then we have the opposite transient right here with the load current dropping

from 5A down to 0A, with a little

spike in voltage returning back to 1.8V regulation fairly quickly.

2:36

The second waveform right here, the second plot shows the control voltage and

the input of the pulse width modulator and

you can see how the red control voltage changes dramatically

during the startup transient and during the step load transient.

The step load transient also includes the waveform of the inductor current.

Which makes a jump from the average value of around zero amps to an average

value above five amps corresponding to the load current of five amps right here.

3:25

Here's the average circuit model for the same example.

Let's see how we arrived at the average circuit model.

Well first of all, the two switches and the gate drivers are replaced

by the average circuit model, the sub-circuit CCM1.

4:06

The rest of the model is exactly the same as the switching circuit model.

We have the LC filter and exactly the same error amplifier right here.

The step load transient is exactly the same as before.

The start up is exactly the same as before.

But notice when we set up the transient simulation, we now include average.lib

library instead of the switching.lib library that we had in the previous case.

One other small detail is that we understand that

the on resistances of the MOSFETs we had in the switching circuit model

are not equal to zero.

Our CCM1 average switch model does not include any losses.

And to make the two the same, we include an on resistance

outside the average switch model in series with inductor, and that all resistance is

the one that is the same, for both the main control FET and the synchronous rectifier.

Allright, so running the transient simulation of this example here,

we get the same set of waveforms and you can see how they look remarkably

similar to the ones we obtained using simulation of the switching circuit model.

In fact it's actually instructive to compare the two.

Here we have a switching circuit simulation on top.

The average circuit simulation on bottom, and you see the waveforms that we

are considering here, Vout, inductor current, inductor current here.

The control voltage here, and how they look remarkably simular.

With one exception - we don't see any ripple in the average circuit simulation

as we have discussed before.

All right, so now that we have established that the average

circuit model can perform transient simulations and

obtain responses that are dynamically very similar to the ones

that we obtained using switching circuit simulation,

we can now use the average circuit model to perform tests

that include AC frequency responses.

6:32

We employ voltage injection using this source,

V-sub-z, that's located between the output of the error amplifier and

the input to the model.

of the pulse width modulator.

That's a voltage injection technique for determining the loop gain.

The loop gain that we find by AC simulation here, is going to be equal to

negative v(y) over v(x) as was discussed earlier

in the course number 3 in the specialization.

In the simulation commands,

of course we use the average.lib library,

we set the frequency range from 50 Hz to 500 kHz

7:57

We may be interested to finding out where the crossover frequency is, and

we can do that using the cursor.

So we can position the cursor at the point for which the response is equal to

zero dB and find out how far the phase response is from -180 degrees.

8:15

We obtain 55 degrees for the phase margin.

As an alternative, or in addition, you can also see

the results of the measurement line in the circuit model we just discussed.

That measurement line can be obtained in the SPICE log file.

Which is available under the view menu, you can simply open the SPICE error log.

The results shown right here,

tell us that the phase margin is 55 degrees or around 55 degrees

at the crossover frequency of 113.5 kilohertz,

which really matches very well the value that we obtained by the cursor.

9:00

Now that we know how to evaluate the loop gain,

the crossover frequency and the phase margin, let's go a step further, and

use a parameter sweep to find out, as a verification step

what happens with the loop gain or the phase margin, cross-over frequency

as the parameters in the circuit change.

So, in particular, may look here,

we are going to step the value of the filter capacitor C1

9:30

from 150uF to 250uF with a step equal to 50uF.

So there's going to be three different values to evaluate the loop gain over.

Otherwise the circuit is exactly the same as before, and

the results are shown right here.

So see now, we have a family of loop gain, magnitude and

phase responses for the three values of the filter capacitor.

And we could also look at the measurement results and

convince ourselves that even though we allow relatively wide tolerance,

of +-20% with respect to the nominal value of filter capacitor our

crossover frequency changes from about 90 kilohertz to about 150 kilohertz.

but the phase margin stays relatively high with

the minimum value of about 50 degrees.

So this is a type of verifications that you may use to evaluate how

tolerances in component values or how changes in operating

10:35

conditions may effect the stability margins or

the performance of your closed-loop voltage regulator.

As a final example, we can also plot the magnitude and

phase responses of the closed-loop output impedance.

Here is the magnitude of the closed-loop output impedance.

You can see on the scale on the left hand side, these are -40 dB down to -100 dB.

So the output impedance of the closed-loop regulator is certainly very small.

11:11

The largest value is obtained at the frequency of about 75kHz and

that value is around 8.5 milliohms

So that gives you a very good idea about how the voltage regulator

will respond to a load transient or

other disturbances on the load side of this voltage regulator.

11:55

You can perform sweeps over parameter values or operating points and

evaluate specifications and performance metrics such as voltage deviations and

response times to the various step-load transients.

In the frequency domain, you can look for crossover frequency, phase and

gain margins.

The output impedance, closed loop, is a measure of how well the regulator responds

to load disturbances in frequency domain and then finally line-to-output responses

can be used to measure how well we reject disturbances in the input voltage.

So overall, we have a powerful tool to evaluate closed-loop

switching power converters using average circuit simulations.