1
\$\begingroup\$

This application note (for the PWM controller I am using, UC3825B) details about error amplifier compensation for the built-in error amplifier.

Error amplifier section of application note

It says it will be compensated to cross 0 dB at (approximately) 1/5th of the switching frequency, 100 kHz (as shown in the second highlight). However, the application note shows that this design switches at 1.5 MHz.

My design using this controller will be switching at 500 kHz, meaning 1/5th is actually 100 kHz.

Now to the actual questions:

  1. Why does it say 100 kHz 0 dB crossing frequency despite one-fifth of 1.5 MHz being 300 kHz?
  2. Can I use these same component values (calculated in the blue highlight) since my design lines up with the one-fifth being 100 kHz?
  3. Regardless of the answer to question #2, can I still use the 3.3 kΩ value for R9 since it is based off of the controller's amp (as stated below the second highlight), and nothing else, to my understanding?
  4. How do the frequencies calculated in the Control to Output Gain section relate to the Error Amplifier Compensation section?

If the answer to question #2 is no, please elaborate on why, and how my understanding is flawed. I'm pretty confused about error amplifier compensation when it comes to calculating the actual component values, and how to choose or find the poles and zeros for different compensator types. Hence why I'm resorting to this section of the application note.

If you need any more information about my design let me know and I will gladly edit the question and provide.

\$\endgroup\$
5
  • \$\begingroup\$ The switching frequency should be large compared to the 0 dB crossing. If not, you need to factor the PWM behavior into the loop and it gets unnecessarily complicated. How much larger? 5X is a generally accepted amount. \$\endgroup\$
    – Mattman944
    Aug 12, 2022 at 21:35
  • \$\begingroup\$ You may want to learn how to break the loop and measure the open-loop response yourself. My power supply experience is limited, so I am not going to attempt to advise you on that. Hopefully one of the experts will arrive. \$\endgroup\$
    – Mattman944
    Aug 12, 2022 at 21:43
  • \$\begingroup\$ @Mattman944 Thanks for your advice, I'm still looking for more direct answers to the four questions I asked so we will wait for more responses like you said. \$\endgroup\$
    – sarrio
    Aug 13, 2022 at 0:19
  • 1
    \$\begingroup\$ @sarrio The document references a very good bit of material from Lloyd Dixon (I think in reference #4.) Have you read through it, yet? (Lloyd Dixon, someone I was fortunate enough to meet in some engineering classes I attended many years ago, is a god of mine. Wonderful person and someone who seriously worked hard to pay-it-forward to others around him. He gave much. Everything he writes is worth some study to learn how he thought about the world.) \$\endgroup\$
    – jonk
    Aug 13, 2022 at 6:11
  • 1
    \$\begingroup\$ Before compensating a converter, you need the control-to-output transfer function which describes the complex response of a stimulus applied to the control pin which is the error amp output in your case. Once you have that plot, you can start discussing crossover selection and compensation. Arbitrarily selecting crossover as a portion of the switching frequency is not the correct way to go in my opinion. Choose \$f_c\$ in relationship with the converter response and the transient performance you need: if 5 kHz are enough, no need to go for 100 kHz because it's 1/5th of \$F_{sw}\$. \$\endgroup\$ Aug 13, 2022 at 7:00

1 Answer 1

2
\$\begingroup\$

Before attempting to compensate a converter, you need to extract the control-to-output transfer function (TF) of the power stage: if a sinusoidal stimulus is applied to the control input of the said converter, how does the signal propagate through the converter to produce an observable response at the output. You have several ways to obtain this TF:

  1. Analytical way: derive a small-signal model of the converter and graph its ac response in terms of magnitude and phase. This is a quite lengthy process which requires an equivalent linear circuit from a switching converter. My last book on the subject covers all the necessary steps for completing the process.

  2. SPICE simulations: if you have an averaged model of the converter you study, then you can use it to extract the ac response of the power stage by first confirming the operating point is correct.

  3. SIMPLIS simulations: SPICE can be used as a frequency-response analyzer (FRA) - see LTspice examples - but it is not very practical in my opinion. SIMPLIS does that natively and you can obtain a Bode plot of the power stage immediately from a switching circuit: no need to resort to an intermediate configuration, just use your cycle-by-cycle model. PSIM also offers this option but in a less easy way I believe.

  4. Bench experiments: build a prototype on the bench and extract the response with a FRA.

It is important to understand what contributes poles and zeroes in a converter and going through 1. is important. This is because production, temperature and operating time affect the transfer function and your role, as a designer, is to neutralize its variability. Therefore, seeing where poles and zeroes are located in an equation is important. Then, you can use 2. or 3. to confirm the response and work on a compensation strategy. In the end, 4. will always be the referee, confirming or negating your hypothesis and calculations.

In your case, I will use one of the 60+ SIMPLIS free templates that I posted on my webpage which, for most of them, work with Elements, the free demo. The schematic of a current-mode (CM) push-pull is shown below:

enter image description here

From this circuit, we obtain an operating point (it is crucial to confirm the converter is properly regulating before considering the response - it is true for SIMPLIS but also SPICE of course) and the ac response of the converter:

enter image description here

Now, what is cool, is that I have automated the compensation elements from a macro in which you enter the desired crossover frequency and the phase margin you want. In this example, I have selected a 10-kHz crossover which is already a good value for a fast-responding converter featuring a 60° phase margin:

enter image description here

The components values around the op-amp are then available from the processed netlist.

Ok, so you now see the process - we've just scratched the surface here - for compensating a converter. Now, let's see your points in particular:

  1. Do not think of a suitable crossover frequency by solely looking at the switching frequency. Crossover and phase margin selection depends on the transient response you need but also from a given robustness you may need at particular frequencies (i.e. input ripple rejection). Besides, crossover selection is often bounded by the converter itself when you have resonances like in a voltage-mode CCM boost or buck-boost converter for instance or if you have a right-half-plane zero (RHPZ) in the power stage TF. A RHPZ sets a limit for the crossover beyond which you'll face instabilities. So pulling out of thin air the crossover frequency based on the switching frequency alone is not a correct approach in my opinion. The more you push crossover, the more noise susceptible your converter becomes and you'll have to deal with issues linked to layout, noise pickup etc. As a preliminary summary, don't push crossover beyond what is really needed for your performance.

  2. No, please go through the process I described as any converter is unique with its own parasitics and components values. With today's tools, the process is truly eased and you can do a lot on the computer before going to the bench.

  3. Please see my answer in 1. and be reasonable with crossover selection.

When all is well stabilized, looking at the transient response is one way to check the converter adequately reacts when subjected to a load step:

enter image description here

\$\endgroup\$
6
  • \$\begingroup\$ Thanks for the very informative response! You mentioned you choose the crossover frequency, which is what I originally thought. What are the side-effects of choosing a crossover frequency significantly lower/higher than 10 kHz in your example? \$\endgroup\$
    – sarrio
    Aug 13, 2022 at 17:25
  • \$\begingroup\$ Disregard the higher than 10 kHz part, I understand that. I'm more concerned about the side-effects of how low you can take the crossover frequency. \$\endgroup\$
    – sarrio
    Aug 13, 2022 at 17:39
  • \$\begingroup\$ Regarding the selection of crossover, please have a look at my APEC 2021 seminar and slide 10 in particular. You'll see that for converters having a resonance in the TF like a buck operated in VM and CCM, you have to select a crossover above this resonance. Otherwise the lack of gain at that frequency won't damp the output impedance and ringing will occur. Otherwise, you can have crossover frequencies down to a few Hz as in a PFC stage for instance. \$\endgroup\$ Aug 14, 2022 at 5:55
  • \$\begingroup\$ Thanks again, very helpful in my understanding so far. Your automation macro lists the variables Ri and N. What are they, and what is the unit "m"? \$\endgroup\$
    – sarrio
    Aug 14, 2022 at 18:59
  • \$\begingroup\$ Ri is the sense resistor and 1:N is the transformer turns ratio. "m" stands for milli like in SPICE notation. \$\endgroup\$ Aug 14, 2022 at 19:06

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.