AVG and RMS in LTSpice?

Dunno if I've grasped the problem, but it reminds me of the time I was sim'ing PWM instability. It's goofy to check the length of hundreds of pulses in LTSpice. So I made a spice circuit to help me spot PWM variations as LTSpice was plotting. Fake circuits to help design real circuits. :) I just call'm helper circuits to get quick analysis.

Perhaps make the electronic equivalent for the behavior you want to observe.

Maybe that helps..

D from BC British Columbia Canada

That's exactly what I've been doing for years. This time it would really clutter things though. Lots of currents to be measure and filtered. I was just wondering whether there was a reasonable math approach.

I just use the mouse to highlight a desired rectangle and release. The chart expands. Then I use ctrl-right-mouse-click, I think, to get the AVG and RMS figures. Something like that... it just pops up in a small dialog box.

Jon

What about an arbitrary voltage source with something like:

V=idt(V(x)-absdelay(V(x),100n))/100n

for a 100ns moving average?

Aren't functions AVG (full average) and AVGX (average over a specified range) available in LTspice?

They're in PSpice.

...Jim Thompson

Nope :-(

I have a really old DOS PSPICE license, maybe time to fire it up again.

Also needed an initial value:

Version 4 SHEET 1 880 680 WIRE 64 48 0 48 WIRE 96 48 64 48 WIRE 0 80 0 48 WIRE 0 192 0 160 WIRE 80 272 0 272 WIRE 112 272 80 272 WIRE 0 304 0 272 WIRE 0 416 0 384 FLAG 0 192 0 FLAG 0 416 0 FLAG 64 48 x FLAG 80 272 avgx SYMBOL voltage 0 64 R0 WINDOW 123 0 0 Left 0 WINDOW 39 0 0 Left 0 SYMATTR InstName V1 SYMATTR Value PULSE(-1 2 50n 0 0 5n 10n) SYMBOL bv 0 288 R0 SYMATTR InstName B1 SYMATTR Value V=idt(V(x)-delay(V(x),100n),V(x)*100n)/100n TEXT 232 264 Left 0 !.tran 200n

Perhaps LTspice's .MEASURE (or .MEAS) statement might be useful to you. There are two ways of using the .meas statement. You can place it in your simulation as a statement and view the results in an error log report or execute the statement in an external text file after the simulation is done.

Example: Place the .meas statement (don't put in the "---") in your schematic (click on the ".op" button in the tool bar with the schematic as the active window):

Thanks, Mark! That may be the ticket here. All I need is a few results, it's ok if I don't really get an efficiency graph. Clicking around in the plot window is too time consuming for rapid-fire optimizations.