Hello all,

I'm trying to find out how to display the average power from a circuit. I'm trying to find out the maximum power output for different load impedances. I'll attach an LT spice file on the post.

I also saw an old thread from 2015 about this same topic, but the trick of clicking alt and left click but it didn't work (power was generally in the micro Watts).

 

Run the simulation. Hold down the ALT key and while keeping it down click on RL. That will give you the waveform of power. Not the average over time. I know there is a way, but it is not in my head now.

 

Hello all,

I'm trying to find out how to display the average power from a circuit. I'm trying to find out the maximum power output for different load impedances. I'll attach an LT spice file on the post.

I also saw an old thread from 2015 about this same topic, but the trick of clicking alt and left click but it didn't work (power was generally in the micro Watts).

After running the simulation, if you hold down the 'Alt' key and left-click on a component, it should add a trace for the instantaneous power absorbed by that component. But if your load is the series combination of the resistor and the capacitor, then that doesn't get you very much.

But notice what this shortcut is actually doing (which you can tell by looking at the trace that it actually adds). It is simply multiplying the voltage across the component by the current through the component. You can do the same thing by adding a trace that is the product of the voltage across your total load and the current through it.

Once you have a trace in the waveform view, you can hold down the Ctl key and left-click on the trace's label and it will bring up a dialog showing the average and integrated values of the trace over the portion that is current displayed.

If you are displaying the average power in the capacitor, you would expect it to be zero over an integral number of periods since it is a purely reactive component. When I run the sim, I'm getting 9.4 µW over the 5 ms sim time. If I look at the average power for the resistor, I get 3.11 mW.

If we ignore the reactive components and consider a circuit that just has the two 1 kΩ resistors in series with a 5 V amplitude sinusoidal voltage, we would expect an average power of 3.125 mW, so that would indicate that either the reactances of the capacitor and inductor are almost perfectly matched, or they are both very small compared to the 2000 Ω total resistance.

If we crank the numbers, we get reactances of:

X_L = 125.7 Ω
X_C = -126.3 Ω

So, it would appear that both conditions are met. The net reactance is about half an ohm.

 

Below is the transient sim of your circuit and then doing ALT/Left-Click on RL, which give a plot of RL's instantaneous power, and then CTRL/Left-Click on the plot title, which shows the average power dissipated in RL of 3.11mW.

If you do the same for V1, you will get double that power, since it's suppling the power dissipated in both RL and Rth (plus the small power dissipated in Xth"s resistance).

What did you do that didn't work?