If I have a mosfet with grounded source that's driving some load to V+, switching the load low side to ground pulsewise, is there some simple way to calculate the fet's power dissipation?
I could measure the voltage and current and multiply-integrate with "analog" components, or do the equivalent with math expressions, but I was wondering if anything like that was built in. Looking at the LT Spice HELP stuff, I don't see anything obvious.
--
John Larkin Highland Technology Inc
www.highlandtechnology.com jlarkin at highlandtechnology dot com
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:
formatting link
formatting link
formatting link
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.
"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:-)
--
"For a successful technology, reality must take precedence
over public relations, for nature cannot be fooled."
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.
--
John Larkin Highland Technology Inc
www.highlandtechnology.com jlarkin at highlandtechnology dot com
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.
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!
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.
--
"For a successful technology, reality must take precedence
over public relations, for nature cannot be fooled."
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.
--
John Larkin Highland Technology Inc
www.highlandtechnology.com jlarkin at highlandtechnology dot com
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
--
"For a successful technology, reality must take precedence
over public relations, for nature cannot be fooled."
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.
ElectronDepot website is not affiliated with any of the manufacturers or service providers discussed here.
All logos and trade names are the property of their respective owners.