Step-by-Step Process to Calculate a DC-to-DC Compensation Network


This article provides designers with an understanding of how DC-to-DC compensation works, why the compensation network is needed, and how one can easily achieve effective results with the right tools. This method uses a simple circuit in LTspice® that is based on a first-order (linear) model of a current-mode buck converter.1 With this circuit, verifying compensation network values can be done without having to perform complex mathematical calculations.


When designing a DC-to-DC converter, components such as FETs, inductors, current sense resistors, and output capacitors are carefully selected to match desired output voltage ripple and transient performance. Following the design of the power stage, closing the loop is necessary. A DC-to-DC power supply has a negative feedback loop that uses an error amplifier (EA). A signal that travels in a negative feedback system could encounter poles and zeros through its path. A single pole will decrease a signal phase by ~90° and will change the gain slope by –20 dB/Dec, while a single zero will add ~90° to the phase and will increase the gain by +20 dB/Dec. If the phase of a signal is decreased by –180°, a negative feedback loop can turn into a positive feedback loop and oscillate. Keeping the loop stable and avoiding oscillations are design criteria for power supplies.

There are two methods for testing for DC-to-DC stability. The first is by frequency response analysis (FRA) in which a Bode plot is created. The second method is a time domain analysis in which a load current transient is performed and the undershoot and overshoot response of the output voltage is observed. To achieve a stable design, make sure the phase stays away from the –180° phase decrease, called phase margin (PM), and this margin should be more than 45°. A 60° phase margin is a good result. A faster response to current load changes is achieved when the bandwidth (BW) of the power supply design is wider. The BW of the power supply is where the 0 dB gain crosses the frequency axis. Also known as the crossover frequency, Fc, the phase at this point is observed to be higher than 45°. The BW of the DC-to-DC converter is a derivative of its switching frequency, Fsw, and is usually in the range of Fsw/10 < Fc < Fsw/5. Fsw/5 means a wider BW and it is harder to achieve. The wider the BW, the lower the phase, so there is a design trade-off. Gain margin (GM) refers to negative gain at Fsw/2 and at –180°, and a –8 dB or higher will provide good attenuation of possible switching noise, or the possibility of gain where phase shifted by –180°. We want to cross the 0 dB point at a –20 dB/Dec slope.

Figure 1. Bode plot showing BW, phase, and gain margins and the crossover frequency, Fc, at 0 dB.
Figure 2. Wider power supply bandwidth has a faster response to current load changes.

The Power Stage LC Filter

The power stage LC filter refers to the inductor and the equivalent output capacitance for a given topology (buck, boost, etc.). Two popular architectures, voltage mode (VM) and current mode (CM), are used for various topologies. The same LC filter behaves differently if used in VM or CM architectures. Keeping it simple, the LC filter used with a VM adds two poles. In CM, there is an additional current sense feedback path that cancels the LC filter double pole. VM is harder to compensate due to the LC double pole that requires more zeros to counter the double pole effect; hence, more components are needed.

Buck VM Architecture and LC Frequency Behavior

The LC filter adds two poles and a zero caused by the equivalent output capacitance CEQ and its equivalent ESR, ESREQ:

Equation 1

Equation 2

The LC filter double pole location is not related to the LC parasitic resistances. Larger inductance and equivalent capacitance values will cause the double pole location to be closer to the origin of the frequency axis at 0 Hz. If CEQ and its ESREQ value are higher, the LC filter zero frequency location will move to the left or closer to 0 Hz. A VM LC filter behavior is shown in Figure 3 and its simulation result in Figure 4. The difference between the red trace and blue trace is the capacitance ESR value, 1 mΩ vs. 100 mΩ. Fr has the same location, as LC values have not changed but the zero location changed due to the change of the ESR value.

Equation 3

Equation 4

Equation 5

Figure 3. A simplified model circuit for a VM buck LC filter behavior.

For VM architecture, the LC filter adds two poles and one zero. The frequency response shape is always the same: 0 dB to –40 dB to –20 dB per decade slope. The location of poles and the zero is dependent on the inductance, total capacitance, and the equivalent capacitance ESR values.

Figure 4. The simulation result of simplified VM buck LC filter behavior.

CM Architecture and LC Frequency Behavior

The LC filter frequency behavior for CM can be simulated by a voltage control current source as shown in Figure 5. The ESR is stepped between two values to show the zero location difference. The pole location for the LC filter in CM buck architecture is given by:

Equation 6

RLOAD is the load resistance that is the ratio of output voltage and current. For example, if the output voltage is 5 V and the load current is 2 A, RLOAD will equal 5 V/2 A = 2.5 Ω. The zero location is set by the equivalent output capacitance and its equivalent ESR. Like in the VM architecture, the two values for 1 mΩ and 100 mΩ ESR are:

Equation 7

Equation 8

Figure 5. A voltage-controlled current source as the model for CM buck; ESR is stepped.

For CM architecture, the LC filter adds one pole and one zero. The frequency response shape is always the same: 0 dB to –20 dB to, again, a 0 dB slope. The frequency location of the pole/zero is dependent on output capacitance, equivalent ESR, and the load values.

The Compensator

The LC filter causes a phase loss. A compensating network is used to provide a phase boost. It adds poles and zeros to the loop to counter the phase lag, or lead, and gain changes that were caused by the LC filter.

Figure 6. Simulation of a CM buck LC filter frequency response shape.

Current-Mode Architecture Compensator

A CM architecture compensator is called a Type 2 compensator. Figure 7 shows a Type 2 compensator. AD8038 is the EA, R2 and R3 are the feedback resistors, and R4 is a resistor on which a frequency is injected into the loop by V1 to perform an FRA. The compensation network is formed from R1, C1, and C2.

Figure 7. A Type 2 compensator modeling in LTspice.

The expected results for the zero/pole and gain:

Equation 9

Equation 10

Equation 11

Equation 12

Gain(bzp) is the gain between the zero and the pole and it is set by the ratio of R1 to R3. The Gain(rz) is the gain at DC. In these calculations, a frequency of 1 Hz was used for the pole at the origin; therefore, the compensator starts at a –20 dB/Dec slope. Figure 8 shows that the simulation results are in close correlation to the computed values.

Figure 8. Type 2 compensator simulation result, pole/zero locations, and slope change.

VM Architecture Compensator

For VM architecture, the compensator has an additional pole/zero combination to counter the additional phase loss of the LC filter. Figure 9 shows a Type 3 compensator network used for VM architecture and Figure 10 shows its frequency response.

Figure 9. A VM architecture compensator, which is also called Type 3 compensator.

C3 and R5 are two additional components that are placed in parallel with the top feedback resistor, R3. The locations of the pole and the zeros for the Type 3 compensator are:

Equation 13

Equation 14

Equation 15

Equation 16

Note that Fz1(EA) and Fz2 are placed at the same frequency. Sometimes, a Type 3-like compensation scheme is used, which uses a single capacitor on the top feedback resistor, so the high frequency pole is excluded, and the compensator slope will continue at 0 dB.

Figure 10. The LTspice AC simulation result of a VM compensator circuit.

Aligning the Time Constants

A method to close the loop is to align the time constants of the LC filter pole/zero with the compensator’s zero/pole so they will cancel each other and provide a total of –20 dB/Dec gain slope.

Figure 11. Poles and zeros alignment of LC filter and compensator for VM and CM.
Figure 12. LTC3981 28 V to 5 V/6 A design schematic where the compensation network is not aligned.
Figure 13. A compensation network is not aligned, the switching frequency is different from the designed one, and a transient test causes oscillation.

Using a First-Order Average Model for Aligning Poles/Zeros

The LTC3891 is a CM controller, which is used for implementing a 28 V to 5 V/6 A. The compensation network, on the ITH pin, is not aligned with the equivalent output capacitance and its total ESR, resulting in oscillations for a transient load test. The measured switching frequency at the output is 23 kHz and not 500 kHz for which it’s designed.

Combining the two circuits of the power stage and compensator together, a linear circuit that models the closed-loop behavior of a CM architecture is formed.

Figure 14. A linear circuit models a CM regulator, and the compensation network is not aligned.
Figure 15. The simulation result of a linear model using an amplifier as an error amp, and the constants are not aligned.

G1 is a voltage-controlled current source. It has a value of 6, which corresponds to a voltage of 1 V at the plus input of G1 that will provide 6 A at its output. The frequency response of this circuit has slope changes at different rates and the 0 dB crossover frequency shows 25° of phase. Therefore, in the time domain, there are oscillations.

To align the time constants, we first need to know CEQ, ESREQ, and RLOAD of the power stage.

Equation 17

Equation 18

Equation 19

R1 is chosen by the designer; here it is chosen as R1 = 11.5 kΩ, the same as R3. R1 × C1(z) = CEQ × RLOAD(p). Solving for C1:

Equation 20

Figure 16. A linear model using an amplifier as the EA after pole/zero alignment.

CEQ × ESREQ (Z) = R1 × C3 (P), the time constant of the compensator’s pole is set by R1 × C3 solving for C3:

Equation 21

A correct simulation result when using this average model shows a –20 dB/Dec slope and phase at 90°. If the result differs, it means that the calculations need to be verified.

One of the drawbacks of using an op amp as the EA is that it does not predict the BW correctly. Still, it is very useful to help in verifying the alignment computation. Increasing the BW can be done by increasing R1 resistance value. If R1 is increased, the compensator capacitors need to be decreased by the same ratio to keep the time constants aligned. There is a limit to how much R1 can be increased as a higher gain means a lower phase margin at 0 dB. The phase is always reported as 90° when the time constants are aligned. The computed values need to be verified using the IC switching model and then bench tested for the transient response.

Figure 17. The result after pole/zero alignment –20 dB/Dec and a high phase value of 90°.
Figure 18. The compensation network on the ITH pin is aligned with the output LC filter.
Figure 19. The simulation result of aligned values of the compensation network and LC filter show stable response to load transient.

This linear model can be made simpler and more accurate by replacing the op amp with another voltage-controlled current source. The LTC3891 data sheet provides the transconductance value, gm = 2 mmho for 1.2 V. As G1 positive input is at 1 V, the new value will be 7.2, as 7.2 A/1.2 V = 6 A/V. A simulation of the new circuit (Figure 20) is shown in Figure 21 and it predicts a BW of 46 kHz.

Figure 20. A simpler alignment circuit using G2 as the error amplifier and its corresponding gm value from the data sheet.

LTpowerCAD predicts a BW of 57 kHz and a phase margin of 52°. The gain plot looks very similar. The phase starts in a very similar manner but is not correctly predicted after 10 kHz.

Right Half Plane Zero (RHPZ)

RHPZ is zero that adds 20 dB of gain and reduces the phase by ~90°, making it impossible to compensate and is a limiting BW factor for topologies like boost, buck-boost, and sepic that work in continuous conduction mode. The frequency location of the RHPZ is calculated by:

Equation 22

Equation 23

Figure 21. A simpler circuit model using G2 as the EA provides a wider BW.
Figure 22. An LTpowerCAD result for LTC3891 design in Figure 18.

Usually, the inductor selection is the only variable in these equations for which a designer can make trade-offs. The RHPZ location limits the BW of the design as the loop needs to be closed at a frequency that is F(RHPZ)/10. The linear model circuits that are offered here do not take that RHPZ into account.

Voltage Mode Buck-Boost Example

The LTC3533 is a VM architecture buck-boost regulator. When in boost mode, the limiting factor will be its RHPZ. The LTC3533 demo board is configured 3.3 V/1.5 A when input is at VIN(MIN) of 2.4 V. In this case, the duty cycle, D, will be D = (Vo – VIN)/Vo = (3.3 – 2.4)/3.3 ≈ 0.27. RLOAD = VOUT/IOUT = 3.3/1.5 = 2.2 Ω.

The RHPZ location can be found by either of its equations:

Equation 24

Equation 25

A safe place to close the loop will be at 8.4 kHz. Rt sets the switching frequency Fsw = 1 MHz. Note that this compensation is a Type 3 like compensation, as RFF is missing, so Cff does not contribute the additional high frequency pole.

The locations for the poles and zeros are:

Equation 26

Equation 27
Equation 28

Equation 29
Equation 30

Equation 31

The double pole location of the LC filter is at 15.65 kHz. The two zeros, Fz1 and FzCff, are placed together at ~9 kHz to counter the poles of the LC filter. Also, the zero that is formed from the LC filter at 967 kHz has a pole to counter its effect at 896 kHz.

Figure 23. An LTC3533 demo board schematic.
Figure 24. A first-order model for VM architecture using an op amp as the EA; LTC3533 demo board values.
Figure 25. A simpler circuit for VM control using a voltage control voltage source.
Figure 26. The result of the simulation of both circuits.

An average LTspice circuit for VM architecture that uses an op amp as the EA can be used to check the alignment of poles and zeros. A simpler circuit can be used by utilizing a voltage control voltage source as the EA. Its gain value is derived from the Error Amp AVOL specified in the data sheet, which is 80 dB. 80 dB = 20log10000. Thus, for the simulation, a value of 10000 is used. The simulation of both circuits provides a very similar solution. The BW has not changed like in the CM circuit simulation. The gain is very similar and the phase is forecasted at 90°, but this only provides information on the correct alignment. There is an additional capacitor of 188 μF and a 0.2 Ω resistor at the output. As seen in Figure 4, a voltage mode LC filter can generate a high Q, especially when ESR and DCR are low in value. To make sure that the LC filter is properly damped, an additional RC is added to the output. It is computed by:

Equation 32


LTspice circuit simulation offers an efficient and reliable way to verify calculations for compensation networks. While the linear model discussed does not include the current sensing element, its signals’ gain, or RHPZ information, the benefits include fast simulation speed and compatibility with various DC-to-DC topologies. Additionally, the output displays a –20 dB/Dec gain slope along with approximately 90° of phase if correct results are achieved.


1Henry J. Zhang. “Modeling and Loop Compensation Design of Switching Mode Power Supplies.” Analog Devices, Inc., January 2015.

LTspice Simulation Files for Power Stages and Average Compensation Models.” Analog Devices, Inc.


Rani Feldman

Rani Feldman joined Analog Devices in 2017 as a senior field applications engineer. Previously, Rani worked for Linear Technology for three years. Rani has a bachelor’s degree in electronics engineering from Afeka College in Israel and holds a master’s degree in business and administration from Holon Institute of Technology in Israel.