Inductor and capacitor loss calculation

Hi SlowWave.

I tried to duplicate you procedure and I got 49mW from the efficiency report but ~45mW using the formula above. see screenshot below.

You may also plot the V(n004,OUT)*I(L1) and do the measurement there.

Just click ctrl+ left click on mouse. however this method will measure the portion of the plot current shown on the screen. you can use this for non steady option.

You may also want to set your trans to only record after steady state is reached. Example is shown below

and then do the ctrl+left click.

onmy trial, I measured 50mW which is close enough on the efficiency report.

in case the result on your machine is different, you want to update your version of LTspice.

my current version is 17.0.32.0.

I hope this helps.

Thanks.

Regards,

PaulDaria

Hi PaulDaria.

Thank you for your support.
My current version is also 17.0.32.0.

I compared your proposed method to the conditions I was examining.
The following [W] is calculated by AVG V*I.

1. default exmaple circuit
     Only the condition of .tran has been changed.   
     
     w/o steady opt 300usec to 500usec is good result.
     w/o steady opt 340usec to 440usec is bad result. (My test results before I asked the question.)

2. L1 Series and Parallel Resistance set to 0
     I changed the following settings from left to right.
     The Efficiency Report (L1) was changed to 0mW.
         

       
       w/o steady opt 300usec to 500usec is also good result.

3. Independent Series and Parallel Resistance
     Add R7 and R8 for Independent Series and Parallel Resistance.
     

     
       L1r (R7+R8) is good result.

///Consideration and questions

Your suggestion (w/o steady opt 300usec to 500usec) was indeed a good result. Did you adjust the start and end times with reference to any of the switching conditions to get this condition?

The efficiency report should be the result calculated from the time axis calculated for the steady option. Do you know why the results calculated by the V*I formula are different, or how to get the same results by formula? It would be nice if there was an option that returns the same calculated result as the steady option.
In other words, I am concerned about the following

I sometimes analyze noise in a single pulse, such as turn-on loss, and I want to accurately estimate where the loss is occurring. Including calculation errors, I have always thought that I would need to look directly at the parasitic resistance loss in situations where there is less than one cycle, and that it would be labor intensive to set up.

I tried the Steady option for the first time this time, and since I was able to accurately estimate the loss in each element in a short time and easily, I thought there must be some way to calculate the same in .meas.
Is there such an option, setting, or formula?

I have a few suggestions that will reduce simulation time and greatly improve accuracy when measuring the dissipation of reactive devices, in particular:

1. Remove the "startup" switch in the .TRAN directive. You don't need to ramp up from zero, when looking at dissipation and efficiency in the steady-state condition. 

2. Add the directives: .ic V(out)=3.35 and .ic I(L1)=839m. These will greatly reduce the start-up transient and further shorten run time.

3. Don't rely on the "steady" switch in the .TRAN directive to set up proper measurement conditions. While convenient, it will introduce errors in measurements. The reason for this is measurement of power, with reactive devices in particular, requires the average V*I product be computed over an integer number of cycles. When "Steady" is used, that's not what you get. Using the LT3684 testjig from the examples folder, "steady" reduced the displayed sweep time to 12.3933μs, which is 10.0955 cycles. This deviation from integer makes a big difference with "spikey" waveforms.

Using ctrl-click in the waveform viewer gave 39.325mW, but using a .MEAS averaging over exactly one cycle gave 48.3854mW. If also run with the "startup" switch and without the .ic directives, the error was worse: 24.985mW from ctrl-click vs. 48.6735mW, because the number of cycles captured was further removed from an integer -> 10.1351.

Try adding the following directives to your schematic:

.tran 100u steady

.ic V(out)=3.35
.ic I(L1)=839m

.MEAS Tmax max time
.MEAS Tstart param Tmax/2
.MEAS T1 when I(L1)=0.85 rise=1 td=Tstart
.MEAS T2 when I(L1)=0.85 rise=2 td=Tstart
.MEAS Fsw param 1/(T2-T1)
.MEAS Cycles param Fsw*Tmax
.MEAS Pind avg V(N004,OUT)*I(L1) from T1 to T2

Incidentally, not mentioned so far is a feature that's enabled when "steady" is used and working: right-click on the inductor after simulation. In the usual pop-up is an additional section called "Simulation Results", which presumably does something similar to .MEAS above as the answer it gave was 49.2mW. This is the same information you get in the Efficiency Report.

The great advantage of using .MEAS for this sort of thing, however, is that when .STEPping variables, you can then plot the .MEAS results afterwards to see the effect. Great if you want to plot things vs. load power or current, for example. It just takes more setting up. In addition, "steady" cannot be used when .STEPping is active.

For situations that don't allow "steady" to be used, i.e. non-ADI parts and those ADI parts that don't support it, you have to use .MEAS anyway, unless you can calculate, in advance, EXACTLY the sweep parameters that give you an integer number of displayed cycles. This may be possible if you're synchronising the switcher with an external clock input, but otherwise practically impossible.

Hope that helps.

Hi TonyCasey.

Thank you for your support.

>The reason for this is measurement of power, with reactive devices in particular, requires the average V*I product be computed over an integer number of cycles.

Yes, I see.
But, I sometimes observe only timing turn-on or turn-off, and I wanted to be able to measure the loss as accurately as possible in a short time.

If it were possible to easily measure the loss of only the parasitic resistance component, it would be simple to do so, but we found that there was no such means.

And in the steady option, the switching time is observed and calculated more strictly internally than the time displayed. I'll try to understand that.

Many thanks,

SlowWave said:

If it were possible to easily measure the loss of only the parasitic resistance component, it would be simple to do so, but we found that there was no such means.

But that's what averaging over one cycle does, by definition: the purely imaginary part doesn't dissipate any power, so what remains is that due to the real part, i.e. the parasitics.

Of course, as you said, if you separate the parasitics outside of the component, it would be simpler, but that's not so easy to do with active devices, which hopefully, always constitute the majority of the loss.

You do have the option of forming your lossy Ls and Cs inside .subckts but shown as regular L and C symbols (to keep your schematic clean and uncluttered), then provided you have enabled the appropriate Control Panel settings in the "Save Defaults" tab (not all enabled by default), you can plot the lossy parts of each component separately. But to get the right answer, you still have to average over an integer number of cycles, if there's an AC component. You would also lose the claimed advantage of LTspice's unique integrated parasitics in terms of the matrix size. However, unless, you have a huge circuit, you'd find it hard to spot any difference.

--

Regards,

Tony