power dissipation in LT Spice

Mouse over the fet to where you get the current probe, then press the ALT key. The probe will change to a little thermometer - click. You will get the power plot. Up at the top will be the nodes (V*I). click on that.

Good advice. I have found the help files in LTspice to be rather deficient, but there are many tutorials and references on-line that I have found when searching for ways to do things. Here are a few:

Something else to remember when calculating power is to choose a period of time long enough to average out, and for repetitive waveforms you should

start and end the sample at zero crossings or peaks. Also let the simulation run long enough for transients to settle, especially when starting with first application of supply voltage from zero. Reactive elements can throw off the measurement. And unless you want instantaneous power at the cursor, use Ctrl-click to get the average and RMS value (or integral) of what you are measuring in the time window you have selected.

Paul

From LTSpice Help:

"Yet another schematic probing technique is to plot the instantaneous power dissipation of a component. To do this, hold down the Alt key and click on the body of the symbol of the component. The instantaneous power dissipation will be plotted as an expression of voltages and currents. It will be plotted on its own scale with the units of Watts. The mouse cursor turns into an icon that looks like a thermometer when it's pointing at a dissipation that can be plotted. You can find the average power dissipation by control-clicking the trace label."

Under wine in linux, it may need . At least, with the window manager I use, it does. (my comment).

"Compute the average or RMS of a trace. The waveform viewer can integrate a trace to obtain the average and RMS value over the displayed region. First zoom the waveform to the region of interest, then move the mouse to the label of the trace, hold down the control key and left mouse click."

RTFM:-)

see

I find it hard to believe you would ask such a question John.

THere must be some other factor you are thinking about that you're not revealing here.

Jamie

if

see

if

see

Because I want to estimate the power dissipation of a mosfet.

Just how hot the fet will get. I don't use Spice very often, and I didn't know about the trick that a couple of people have pointed out. Power-vs-time is interesting, but it's still not average power.

The last time I actually did real calculus was to get the equation for fet power dissipation in a situation with a linear load. Now I'm driving time-varying nonlinear loads.

I can probably get close enough with just SWAG arithmetic for this application, but I was wondering if there was some simple way to do it in LT Spice.

I might still build a "wattmeter" in LT Spice. A shunt resistor, a couple of VCVSs, a multiplier, an integrator.

if

see

power

application,

Ok, Joe has explain the thermometer thingamagic via ATL-LeftClick in the schematic. Now you have a plot power-versus-time. Mouse over its expression on the top of the waveform window -> CTRL-LeftClick and ... voila. A little text window open that contains average power and so other information.

You have to wait until the simulation stopped, such integration will not working while running.

if

see

power

application,

I've learn to use a calculator years before I even touched on the use of spice.

I know spice is a nice tool to use and at times, it could cause you brain damage, or lack of I should say. If you don't exercise it a bit with the connectivity from the neurons down to the tips of your fingers via the path ways you were born with, pushing those little keys, you'll end up like slow-Man, all talk and no walk!

Jamie

--^^^^^^^^^

This should be ctrl-click for the average power.

It was too early in the morning (or is that late in the work day) to be posting

Averaging the products of individual samples, however, is.

You can average a power waveform (see previous post), or use a .meas statement, like:

.meas pwr tran avg(Id(M1)*V(N002))

which averages the products of individual samples.

No need to simulate a wattmeter.

You can do true and apparent power, hence power factor, using .meas statements, too.

To view results, view SPICE error log.

It's all in the manual.

This example should explain. Deliberately nonlinear.

Version 4 SHEET 1 880 680 WIRE 240 -16 80 -16 WIRE 80 0 80 -16 WIRE 240 16 240 -16 WIRE 240 112 240 96 WIRE 192 192 64 192 WIRE 64 208 64 192 WIRE 64 304 64 288 WIRE 160 304 64 304 WIRE 240 304 240 208 WIRE 240 304 160 304 WIRE 160 320 160 304 FLAG 80 80 0 FLAG 160 320 0 SYMBOL nmos 192 112 R0 SYMATTR InstName M1 SYMBOL res 224 0 R0 SYMATTR InstName R1 SYMATTR Value 100 SYMBOL voltage 64 192 R0 WINDOW 123 0 0 Left 2 WINDOW 39 0 0 Left 2 SYMATTR InstName V1 SYMATTR Value 5 SYMBOL voltage 80 -16 R0 WINDOW 123 0 0 Left 2 WINDOW 39 0 0 Left 2 SYMATTR InstName V2 SYMATTR Value SINE(0 10 60) TEXT 30 338 Left 2 !.tran 1 TEXT -320 152 Left 2 !.meas pwr tran avg(Id(M1)*V(N002)) TEXT -320 104 Left 2 !.meas rmsv tran rms(V(N002)) TEXT -320 80 Left 2 !.meas rmsi tran rms(Id(M1)) TEXT -320 128 Left 2 !.meas appar param rmsv*rmsi TEXT -320 176 Left 2 !.meas pf param pwr/appar

OK, all that works:

Thanks.

I did, but it turns out to be buried in "Trace Selection." It's easier to ask here.

to

"analog"

if

don't see

know

power

application,

Fred's advice got me there. Cool.

In the pic I posted, note that I simulated for 51 us. If I simulate for 50 us, it takes minutes to run. At 51, it finishes instantly!

I was working WBOC this morning, Without Benefit of Coffee. I'm full of Peets now and things are clear.

The target is to make some fast 7.5 KW pulses. Soon.

Yup. Same here.

Specifying max timestep 10ns, it runs fast, 1ns, it starts at 6us/s, slows down to about 3fs/s, then speeds up again. I've notice similar slowdowns around fast edges before.

to

"analog"

wondering if

don't see

know

power

application,

So it works when it's one card short of a full deck, just not two cards. ;)

Cheers

Phil Hobbs

Cheers

us,

Takes longer to simulate less time!

to

edges

I wonder why it doesn't have a box for min timestep. I've used (and written) other simulators that did, allowed you to deliberately trade accuracy against sim speed.

to

"analog"

wondering if

don't see

know

power

application,

of

us,

There's always a Joker.

us,

down to

edges

Results using 50us, 1ns timestep:

pwr: AVG(id(m1)*v(n002))=1.58253 FROM 0 TO 5e-005 rmsv: RMS(v(n002))=17.5187 FROM 0 TO 5e-005 rmsi: RMS(id(m1))=9.48311 FROM 0 TO 5e-005 appar: rmsv*rmsi=166.132 pf: pwr/appar=0.00952577

In that case I'd consider negative gate drive for the turn off, and a drive with some serious gusto, and maybe +12V and -10V. Maybe even a peaker. Plus a blast shield for the FETs.