Temperature measurement in LTspice

[alec_t]

the load should be more resistive due to the PFC function

There is no PFC function in the post#37 circuit, which is the one I was referring to in post #38.

 

[mading2018]

There is no PFC function in the post#37 circuit, which is the one I was referring to in post #38.

Aha, I see. I meant post #36, with the boost PFC converter. Sorry that I was unclear.

 

[ronsimpson]

Quoting Mading2018:

"the voltage and current over the component" is only right for certain parts. It can not be right for capacitors or inductors.
If I make a coil with "magic gold wire" that has no resistance there will be no power loss. I can put 1000V and 10A on the coil for 10us then -500V and 10A for 20uS and there is no power loss. SPICE sees 1000*10 and -500*10 and generates very large "power" numbers.

Same thing for capacitors. Perfect SPICE capacitors with out resistance will not have loose power.

I think to find the power loss in L or C you must know the internal resistance and add it outside the L or C (in SPICE). Then find the power loss in that resistor by the V*I. I know from real world PWM that If I put 10W in and get 9W out that I am missing 1W. (efficiency)

A PFC is hard to measure. I would put 200VDC in and measure 400V out. Find DC power in and DC power out. This is close to the right answer.
You should be measuring 2 to 4 watts loss in the inductor. I have build these things. The input/output capacitors should have some small fraction of a watt loss. I have measured them. Not SPICE parts but real parts. I know if I get too much power loss in a cap then I choose a different cap with better Internal Resistance and the temperature drops. The efficiency goes up.

In an incuctor there is more power loss than I^2*R. There is core loss. I think SPICE can find that but it gets very complicated.

While I am complaining, in a PFC (that is working correctly) the duty cycle is different depending on the phase of the power line voltage. So what " during one cycle" are we talking about. If you measure input power at a "one cycle" that is at the power line "zero crossing" the input power is zero, while the output power is 400 watts. The efficiency looks real good.

 

[crutschow]

My faith in Spice's power calculations is being tested .
It seems your circuit can achieve over-unity!! If you set the sim period to 10mS and start saving data at 2mS, then over the 8mS interval the average 'power' provided by V1 is ~791.9W but the average power dissipated in R1 is 795.7W .
[Explainable by the load seen by V1 being primarily inductive]

Don't understand your results.
My simulation shows the opposite.
It has the output power about 2W less than the input power.

 

[crutschow]

SPICE sees 1000*10 and -500*10 and generates very large "power" numbers.

It calculates the VA numbers, which is apparent power.
It's the average of those calculations over an integral number of complete waveform cycles that's the real power.

 

[alec_t]

My simulation shows the opposite.

Curiouser and curiouser, as Alice would have said. We must have something different in our settings.


Edit:
I wonder if processor clock speed is a factor?

 

[ronsimpson]

It's the average of those calculations over an integral number of complete waveform cycles that's the real power.

On a capacitor, if the start voltage is the same as the end voltage then the flow of electrons must equal zero. (current average =0)
On a inductor, the average voltage=0. (SPICE inductor) If the start current = end current then the average voltage = 0

In a PFC you will have trouble measuring one cycle of the PWM. I think you will need to measure over one power line cycle. (or 1/2 cycle) The point is; the input can be as low as 0 or as high as the peak of the power line. The output voltage does not hold constant. It normally varies 20 volts. If you pick a PWM cycle near the time of the power line crossing zero you might have a moment in time where the input power is 1 watt and the output power is 100 watts. BUT At the peak of the power line, the input might be 150 watts while the output might be 98 watts. Two people measuring power over one PWM cycle must agree on which cycle they are measuring.

Also PFC takes about 100mS to get up and running stable. Measuring power in the first 10mS will not get a stable answer. The output capacitors are charging at 10mS so the "energy" measurement is giving how much power is entering the output caps. OR Most PFCs overshoot. Measuring near the over shoot time will give bad answers.

 

[crutschow]

We must have something different in our settings.

Which LTspice version are you using?

 

[crutschow]

Two people measuring power over one PWM cycle must agree on which cycle they are measuring.

The error is reduced if you average the value over many integral waveform cycles.

 

[alec_t]

Which LTspice version are you using?

XV11.
I tried with and without 'Skip initial operating point solution' enabled, but that made no difference.
In Control Panel/Spice I do have Trtol set to 7, if that's relevant.

Edit: Yup, that's what accounts for the difference. With Trtol=1 I duplicate your result, Crutschow.

 

[crutschow]

XV11

Same one I used.

 

[mading2018]

I tried with and without 'Skip initial operating point solution' enabled, but that made no difference.
In Control Panel/Spice I do have Trtol set to 7, if that's relevant.

Edit: Yup, that's what accounts for the difference. With Trtol=1 I duplicate your result, Crutschow.

Would 10 ms be enough to run the simulation as it is DC in the input?
And for my PFC circuit, I can ran 100ms, due to it takes time for the PFC to get stable.

 

[alec_t]

I would think the longer you run the simulation the closer you will get to a stable situation. However, as Crutschow has pointed out, LTS is computing apparent power, not real power, for reactive components.

 

[mading2018]

I would think the longer you run the simulation the closer you will get to a stable situation. However, as Crutschow has pointed out, LTS is computing apparent power, not real power, for reactive components.

Yes, that's true. But if I only measuring power losses for the other components, diodes, mosfets and resistor, I can obtain the real power.
So I have decided to skip to measure the inductors and capacitors.

BUT what I understand, from Crutschow comments,

It calculates the VA numbers, which is apparent power.
It's the average of those calculations over an integral number of complete waveform cycles that's the real power.

Is that average the same as we can read from the simulation window when we are measuring power dissipation?

 

[crutschow]

..........
Is that average the same as we can read from the simulation window when we are measuring power dissipation?

Yes, that's the same average.
LTspice calculates the instantaneous V*A in the plot.
If you take the average of that over an integral number of cycles, you will get the averaged real power, the same as you would measure with a meter.

Look at the LTspice simulation below of a simple RC circuit powered by a sinewave.
Note that even though the resistor voltage is only about 1/2 the input voltage, the average power over an integral number of cycles for the V1 source [V(IN)*I(V1)] is the same as the resistor average power (since all the source power is dissipated in the resistance).
And the capacitor average power, as expected, is essentially zero.

 

[ronsimpson]

And the capacitor average power, as expected, is essentially zero

CrutsChow,
Please run the same test but add a 50V dc to the bottom of V1. (or add a 50V offset to V1)
I want to see what the V1*IC1 looks like with AC+DC on it.
On my Pi so no SPICE today.

 

[crutschow]

Here you go:

 

[ronsimpson]

Here you go:

Wow. You did it. I thought I did this a week ago and got many watts.
I can see that current spends 50% positive and 50% negative. That works.
Voltage spends more time positive. I though the answer, average of V*I, would be positive large.

Now my head hurts.

 

[alok1982]

Great to see this thread live again!

 

[MikeMl]

Look at this posting, which I came up with without even seeing this one. Great minds think alike...