On Tue, Apr 8, 2025 at 10:53 AM, Dennis wrote:
Excellent work.
?
This comment from me, below, affects only few of you, so most of you can ignore it.
?
The simulation has considerable "Trap Ringing" (or "Trap Oscillation") at the MOSFET's drain current when the MOSFET switches off.? That is not unusual, and Mike Engelhardt used a situation like this to illustrate Trap Ringing.? (In case you don't know, "Trap Ringing" has bothered SPICE users since the beginning of time.? It is a mathematical artifact.)
?
The ringing is evident if you use the "Trapezoidal" integration method.? "Trapezoidal" was the SPICE default, but it is not LTspice's default which has the improved "Modified Trap" method.? Either "Modified Trap" or "Gear" methods eliminate the appearance of the Trap Ringing.? Go to Control Panel (Settings) > SPICE tab, and check the buttons under Default Integration Method.? Unless you changed it, yours is probably set to "Modified Trap" already, and you are good.
?
I happen to have my LTspice set to the old default "Trapezoidal" method even though it can be problematic compared to "Modified Trap", because I actually want to see Trap Ringing when it happens.? Most LTspice users will not want to do that.
?
LTspice's "Modified Trap" method is not really a distinct integration method; it is actually a post-processing nonlinear filter that removes 99% of Trap Ringing's visible artifacts.
?
Unrelated:? On the computer I used today, LTspice could not read Dennis's plot defaults (*.plt) file included with this simulation.? ?It reported "Plot setup file syntax Error".? I guess someone at Analog Devices must have modified the .PLT file syntax.? I had to enter the traces manually.? ?But that was not a problem, because the valuable results in this simulation are in the Error Log file, not the plotted waveforms.? Press Ctrl-L from the schematic window to see those results in the Error Log.
?
Andy
?
