# LTC1871 - Can I simulation AC analysis in LTSpice?

I would like to design a power supply with LTC1871 and my question is can I simulation AC analysis in LTSpice with this IC?

Best regards

## Top Replies

Parents

The technique to measure frequency response of a switching power converter has been provided in the FAQ section of LTspice documentation labelled "How to get a Bode Plot from a SMPS".  The steps are (taken from LTspice doc):

Step 1: 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.

Step 2: 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.

Step 3: 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.

Step 4: 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.

Step 5: 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.

Step 6: 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 plotted. so right click again and execute menu command "Visible Traces" and then select gain.

The technique to measure frequency response of a switching power converter has been provided in the FAQ section of LTspice documentation labelled "How to get a Bode Plot from a SMPS".  The steps are (taken from LTspice doc):

Step 1: 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.

Step 2: 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.

Step 3: 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.

Step 4: 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.

Step 5: 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.

Step 6: 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 plotted. so right click again and execute menu command "Visible Traces" and then select gain.

Children
No Data