# LTspice: Extracting Switch Mode Power Supply Loop Gain in Simulation and Why You Usually Don't Need To

Mar 3rd 2014

The gain of a negative feedback loop needs to fall with frequency below unity before too much phase shift occurs unless your aim actually is to make an oscillator[1]. This idea can be applied to the stability analysis of a Switch Mode Power Supply(SMPS). Even though a SMPS is an intrinsically non-linear circuit with no small- signal linear equivalent circuit, there typically is an analog feedback loop operating on the filtered, switched output.

There are two issues involved in determining the loop gain of a SMPS (i) obtaining the open loop gain from the closed loop system and (ii) ignoring the switching waveform by averaging over a switching cycle and/or using Fourier analysis to ignore the switching frequency components. The first issue is common to most stability analysis of feedback loops. Stability analysis is based on the open loop response but if you break the feedback loop to measure open loop response directly, the circuit doesn't work anymore which was why feedback was used in the first place. The second issue arises from the fact that a SMPS is an intrinsically non-linear circuit and linear feedback theory is basically restricted to the hypothetical waveform averaged over a switching cycle.

Determining the open loop response of a linear, closed loop system is a problem solved well by Middlebrook's method[2]. That method uses test signals injected into the closed loop system to independently solve for the voltage and current gains. These two gains are then convoluted together to get the true loop gain. If a point in the feedback loop can be identified where a low impedance drives a high impedance, then the current gain is zero and it is sufficient to measure only the voltage gain and identify that as the loop gain. Such a point can normally be found in a SMPS since you have a power supply output driving an error amplifier input.

Laboratory measurement of a SMPS loop gain is automated with commercial instrumentation pioneered by Venable Corporation and now also available from other companies. The technique of using injected test signals and Fourier analysis is called Frequency Response Analysis(FRA). While this method is routine in the lab, not everyone is aware of how to use it simulation. This article explains how to do FRA in LTspice IV. The method uses the voltage gain part of the Middlebrook method, .measure statements to do the Fourier transform, a step statement to sweep frequency, and the feature in LTspice that allows one to plot the results of .measure statements. In reading through the steps below, you might want to refer to the working FRA examples that are part of the general LTspice IV release typically installed in directory

C:\Program Files\LTC\LTspiceIV\examples\Educational\FRA\

- Identify a point in the SMPS feed back loop where a low impedance source is driving a high impedance input. Two places are useful for this, either in series with the feedback pin of the SMPS controller or between the output to the top of the resistor divider going to the feedback pin.
- Insert a voltage source here. This will be a time-domain sine wave that perturbs the feedback loop. Give it a value of "SINE(0 10m {Freq})" The choice of amplitude(here 10mV) will impact accuracy and the signal to noise of the method. The smaller the amplitude, the lower the signal to noise. But if the amplitude is too large, the system is not operating linearly and frequency response becomes less relevant since the frequencies are no longer independent.
- Label the nodes to either end of this voltage source "A" and "B" The direction of feedback should be from node A to node B. For example, if the voltage source is connected directly to the feedback pin, node B is the feedback pin and node A is the one on the other side of the voltage source.
- Paste the following .measure statements on the schematic as a SPICE directive:

*.meas Aavg avg V(a)** .meas Bavg avg V(b)** .meas Are avg (V(a)-Aavg)*cos(360*time*Freq)** .meas Aim avg -(V(a)-Aavg)*sin(360*time*Freq)** .meas Bre avg (V(b)-Bavg)*cos(360*time*Freq)** .meas Bim avg -(V(b)-Bavg)*sin(360*time*Freq)** .meas GainMag param 20*log10(hypot(Are,Aim)/hypot(Bre,Bim))** .meas GainPhi param mod(atan2(Aim,Are)-atan2(Bim,Bre)+180,360)-180*

These .measure statements perform the Fourier transform of nodes A and B and then compute the ratio of the resultant complex voltages. The result is the complex open loop gain of the system. The magnitude is given by GainMag in dB and phase as GainPhi in degrees.

- Paste the following on the simulation command on the schematic as a SPICE directive:

*.param t0=.2m** .tran 0 {t0+10/freq} {t0}*

Parameter t0 is the length of time required for the system to come to steady state. You will probably have to run a few simulations to determine an appropriate value for t0. It occurs as the third parameter on the .tran command, meaning is it the time the simulator should start saving data. This prevents the .meas statements of Step 4 from using this data in the analysis. This is done because initial transient conditions might not be operating within the small perturbations from regulation that could be considered small signal response.

Notice that t0 appears in both the 2nd and 3rd parameters of the .tran command. The 2nd parameter is the stop time. The difference between start and stop times has been chosen as 10/freq, i.e., an integral number of perturbation cycles. Ideally, the Fourier analysis would be done over a period that is both an integral number of perturbation cycles and switching cycles, but his isn't always possible. Since loop gain must drop to less than unity at a frequency that is a fraction of the switching frequency, there are always more switching cycles than perturbation cycles and an integral number of perturbation cycles is used with the hope the error from a non-integral number of switching cycles will be small since many switching cycles are included.

- Choose which frequency or frequencies at which to perform the analysis. To do a single frequency, simply add this SPICE directive:

* .param Freq=15K*

and run the simulation. The output of the .meas statements are in the error log which you can view after running the simulation with menu command View=>SPICE Error Log. You can run the simulation at multiple frequencies by placing the following SPICE directive on the schematic:* .step oct param freq 50K 100K 5*

This directive tells LTspice to run the simulation at frequencies from 50kHz to 100kHz using 5 points per octave. To plot this as a Bode plot, after the simulations complete, execute menu command View=>SPICE Error Log and then right click menu "Plot .step'ed .meas data" At this point, the Bode plot will not have any data ploted. so right click again and execute menu command "Visible Traces" and then select gain.

Armed with the above technique, one might feel ready to go and conquer SMPS design with Bode analysis of the feedback loop. I understand the temptation. It'd be rewarding if one could traverse the feedback loop identifying the components that gave rise to the poles and zeros, strategize which zeros to move to cancel which poles, and synthesize component values for the compensation network components to achieve a stable feedback loop. But that's pretty much exactly what you can't do with this technique or any other frequency domain technique. Let me explain why.

Let's consider a typical fixed-frequency, peak-current mode switcher such as that in ...\LTspiceIV\examples\Educational\FRA\Eg3.asc

The controller uses a flip-flop which is set by a clock pulse and turns on the switch which ramps the inductor current up. Once the peak switch current is proportional to the voltage on the output of the error amplifier, the flip-flop is reset, the switch turns off and the controller sits idle while until the next clock pulse sets the flip-flop again. Since average current is proportional to peak current up to a geometrical factor, if we average over one clock cycle this flip-flop controlled-switch behaves like a transconductance. That is the current through the switch is proportional to the voltage on the output of the error amplifier. Now if continue on along the feedback path, we have the inductor in series with the switch current. Since the switch is a current source, the series impedance of the inductor, even though it is reactive, causes no phase shift. This is actually the point to current-mode control and why you buy that controller. Continuing on the feedback path, we are now at the output of the SMPS. The output filter capacitor(C4) gives rise to one pole. The output is then divided by the feedback resistive divider and compared to a reference voltage at the feedback pin. The difference between the divided output and the reference voltage is the error voltage. This error voltage is amplified the the error amplifier to be a current which flows out of the error amplifier. But it is the voltage on the output of the error amplier and not the current flowing out of it that determines switch current so to complete traversing the feedback loop, we need to convert that current to a voltage. We could do that with a resistor and that would work, but a much better idea is to use a capacitor(C1) because that will maximize the open loop DC gain to keep the output regulated to a stiff voltage. That capacitor makes a second pole.

Now, since each pole can cause a phase shift infinitesimally close to 90° and the controller must cause some additional delay, one might think that some circuit design is necessary to ensure a stable feedback loop. But that's not really the case particularly if one is using an aluminum electrolytic cap output filter capacitor because it has ESR and that will put a zero in the response. Also, since we buy compensation cap C1 a series resistor, R1, that also puts another zero in the response. Further, the delay from the controller is a very small fraction of the switching frequency. At the loop crossover frequency and below, that delay is negligible. This all means that the loop is stable and it isn't possible to synthesize component values since the loop is stable for all component values. This argument basically is pointing out that as soon as the signal regulated by the feedback loop of a current mode SMPS is well- described by the current averaged over one switching cycle, that loop is stable.

If the output filter cap isn't an aluminum electrolytic but a ceramic capacitor, the ESR of a ceramic capacitor isn't high enough to substantially impact the stability of the SMPS. So the loop response, per the previous discussion, would now be two poles and one zero so it should still be stable independent of the specific component values of the output filter cap or RC circuit attached to the error amplifier output. But it would be appropriate to discuss the limits of applicability of the above analysis. There is an effect that degrades from the accuracy of the above description of current mode SMPS stability. The average current isn't proportional to the peak current over variation of output voltage because the duty cycle, and hence ripple current, changes with output voltage so the same peak current that trips the controller flip-flop does not give the same average current over changes in output voltage. This means that the transfer function from the voltage on the output of the error amplifier to the current flowing into the inductor isn't perfectly described as a transconductance, but a transconductance shunted with some real impedance. This impedance is typically several Ohms, which while very large compared to the on resistance of a MOSFET, it is less than infinite. This is not desirable from a stability point of view since the inductor is no longer fed from a current source and its reactance can cause some phase shift. This situation is further degraded by slope compensation. Slope compensation is the fix for a subharmonic oscillation that occurs in fixed frequency current mode controllers operating at high duty cycle. The technique entails adding a spoofed current to the measured switch current and using that quantity to reset the controller's flip-flop. The impact of using a quantity other than current to reset the flip-flop reduces the impedance of the current source feeding the inductor so the inductor's reactance causes yet more phase shift.

By and large, I find it pretty hard to make a current-mode SMPS unstable. For example, if you use an inductance value that is too high by an order of magnitude or two, then inductor ripple curent becomes very small and the spoofed current of the slope compenstation controls the flip-flop reset. That will reduce the impedance of the switched source driving this inductance to the impedance of the MOSFET Rds(on) so the inductor creates another pole in the loop and that causes instablity. But in that situation, even though you're using a current mode controller, the power supply is actually running in voltage mode. Small signal linear analysis of voltage mode power supplies is quite useful because unless the feedback loop has been contrived to cancel one of the poles, the power supply will oscilate and may blow itself up the first time it is turned on. Current-mode supplies are quite different. While it is possible to do small-signal linear analsys of a current-mode switcher, there just isn't much engineering to be accomplished with the method since the feedback loop is stable as long as the power supply really is operating in current mode.

The last advise I can offer answers how one can be sure that a SMPS is stable and operating in current mode. The answer is to start with the schematic on the front page of the datasheet. The critical information there are the inductance value, output filter capacitance, and external compensation component values. Some datasheets give equations for computing these values, but I just start with those values and adjust using time domain simulation to evaluate the response. After all, the whole point of frequency domain analysis is to improve the time domain response. With current-mode switchers, it usually more direct to jump right to time-domain simulation to check overshoot since stablity has already been achived.

1] The discussion is restricted to minimum-phase systems.

2] R. David Middlebrook, "Measurement of Loop Gain in Feedback Systems", International Journal of Electronics (vol 38, no. 4, pages 485-512, April 1975).

## Software

### LTspice

LTspice^{®} software is a powerful, fast and free simulation tool, schematic capture and waveform viewer with enhancements and models for improving the simulation of switching regulators. Click here to download LTspice

To launch a ready to run LTspice demonstration circuit for this part:

**Step 1:**If you have not installed LTspice on this computer, download and install LTspice**Step 2:**Once LTspice is installed, click on the link(s) below to launch the simulation

**Step 3:**If LTspice does not automatically open after clicking the link above, you can instead run the simulation by right clicking on the link and selecting "Save Target As." After saving the file to your computer, start LTspice and open the demonstration circuit by selecting 'Open' from the 'File' menu

To explore other ready to run LTspice demonstration circuits, please visit our Demo Circuits Collection.

### View More LTspice Solutions

**View All** - List View