Engineering AM-AM and AM-PM graph generation in LTSpice

[nomi114]

Homework Statement

How can we generate amplitude-to-amplitude and amplitude-to-phase graphs in LTSpice?

Relevant Equations

NA

Greetings to all,

I am writing with a question regarding graph generation in LTSpice. I am using LTSpice XVII and am trying to plot AM-AM and AM-PM characterization for a power amplifier, but I haven't been successful yet, likely due to my lack of practice with this specific analysis. I have been using a square wave input at 8.2 MHz as the voltage waveform for my power amplifier. It is said that for a switching amplifier like Class-D, the AM-AM / AM-PM (amplitude-to-amplitude and amplitude-to-phase) plot is often more straightforward to simulate and relates directly to amplitude accuracy. This checks how the output power and signal phase change as you increase the input power.

I would greatly appreciate your assistance in this matter. For your reference, I have attached the schematic file as a .text file. Thank you in advance for your kind help.

 

[Baluncore]

This checks how the output power and signal phase change as you increase the input power.

It is difficult to do those simulated tests because you have two trapezoidal inputs, with feedback from the amplifier output to the input bias. Changes of the input power will require a settling time for the bias before a reading can be made, so the plots cannot be done in a single sweep.

You will need to .STEP an input amplitude parameter, then use .MEASure to extract the output information from the plot for each step.

 

[nomi114]

Thank you so much for your kind reply. If you don't mind, could you please help me understand how to implement these commands in my schematic? I have tried but was unsuccessful. I am currently stuck and would highly appreciate your guidance.
Thank you in advance for your cooperation.

 

[Baluncore]

Modified the signal input, so only one parameter is needed.
I have given you a .STEP command. For vin = 1.0v to 3.5v step 0.5v
Experiment with the .asc and .plt files attached. Notes in the top left corner.
Here is the plot produced by the .STEP, showing amplitude and phase changes for different input amplitudes.
Is the limiting due to your bias adjustment or saturation of the PA ?

 

[nomi114]

Thank you so much, dear Sir, for your kind and prompt response. Here, I would like to inquire about one question: there is a small step phase variation in each (almost) output signal. I am a little bit confused. Why is there this variation? Is this a circuitry issue or what.........? Thanks in advance for your kindness.

 

[Baluncore]

Here, I would like to inquire about one question: there is a small step phase variation in each (almost) output signal. I am a little bit confused. Why is there this variation?

I assumed it was when your bias control circuit began to regulate, or the output voltage saturated. Maybe change the step parameters to focus on that phase and amplitude transition. You can investigate why using LTspice.

To generate the AM-AM and AM-PM graphs.
First view the VP1 input signal only, you can adjust the .TRAN "time to start storing data" to bring the VP1 rising edge, to zero volts, at zero time. Record the trace colours and input voltages.
Then view the LOAD output signal only, zoom in, to read and record the amplitude of each colour trace, and the rising edge zero crossing time for each trace.
From that information and the signal period, you can generate the AM-AM and AM-PM graphs.

 

[nomi114]

Dear Sir, Bundle of thanks for your guidance. I have followed your instruction but am still a little bit confused about drawing these graphs. I used the following commands for the simulation at first:

.step param Pin -20 20 1; Sweep input power from -20 to +20 dBm

.meas Vout_max MAX V(Load)
.meas Vin_max MAX V(VP1)
.meas phase_delay TRIG V(VP1)=0 RISE=1 TARG V(Load)=0 RISE=1

Then I have checked the Error Log and Plot .step'ed .meas data.

But it is taking a long time; I think it is beyond my computer's (processor) capabilities. About 20 minutes passed; the simulation is still in progress. Based on your previous simulation graphs, can I ask for a little favor, please? Can you check if I am on the right track, or can you generate this graph at your computer, please? If it will not bother you.

 

[nomi114]

By using these commands, I have the following graphs. I am not sure how it can be defined or if it's correct or not. Need suggestions, please.

 

[Baluncore]

.step param Pin -20 20 1; Sweep input power from -20 to +20 dBm

You are sweeping Pin (whatever that is) from -20v to +20v in steps of 1v, which is 41 trace sweeps.
To perform a logarithmic sweep you must include the keyword OCT.
Do not use OCT with sweeps from negative, through zero, to positive.
Read the LTspice help page for .STEP

Get the logarithmic steps functioning before you try to .MEASure.
Try to .STEP from 0.1v to 3.3v with one sweep per octave.
.STEP OCT PARAM Pin 0.1 3.3 1 ; gives 0.1, 0.2, 0.4, 0.8, 1.6, 3.2
.STEP OCT PARAM Pin 0.1 3.3 2 ; gives 0.1, 0.142, 0.2, 0.283, 0.4, 0.566, .... , 3.2

 

[nomi114]

sure sir, let me try this.

 

[Baluncore]

I notice that for small VP1 drive amplitudes, ±2 volt and below, the MOSFETs are not turning off, but are conducting large continuous currents. That must be avoided as it will result in high device power dissipation, in this case, over 660 watt.

The high power linear, rather than efficient switching mode, of MOSFET operation, explains why the significant output phase step occurs below about ±2 volt.

By hovering the mouse over the device body on the schematic, you can display the average device power during the last simulation run. Power can be plotted, by left-clicking on the device, while holding down the ALT key. It will make more sense if you disable the .STEP function first.