X-Mailer: Mozilla 4.79 [en] (Win98; U)
Subject: Re: SPICE and amp stability
NNTP-Posting-Date: Wed, 20 Nov 2002 17:39:06 GMT
Organization: AT&T Broadband
Date: Wed, 20 Nov 2002 17:39:06 GMT
Jim Thompson, Mike Engelhardt, Kevin Aylward, Walter Harley wrote:
>>>> Or is there some more correct way to determine the loop
>>> You have to look at the *loop* gain. This is the open loop gain
>>> around the *feedback* path. This involves setting up a circuit
>>> such that the opamp has a closed loop for dc (or very, very low
>>> frequencies), but open loop for the main plot. This is so the
>>> amp will bias correctly. The easist way to see how this is done
>>> is to run my SuperSpice LoopCutter.sss example:-).
>> This is a poor way of doing this. All you have to do insert a
>> floating AC voltage source in series with the feedback at in front
>> of a high impedance point of the circuit, typically the opamp input.
Er, shouldn't that be a floating voltage source inserted in series
between a very low impedance source and the finite impedance branch
to which it was formerly connected? (Or the dual method with a
current source, of course.)
>> Then do your .AC analysis, and plot the ratio of complex voltages
>> to either side of the voltage source. This method also is a good
>> one for bench use, called either a frequency response analysis or
> If you're using PSpice, you can download, from my website, my
> "Loopgain" part. This performs two passes, one with voltage drive,
> and one with current drive, then computes gain and phase; all done
> without perturbing the loop.
This is general method that works regardless of the relative
impedances at the insertion point within the loop to be measured,
although most circuits have a convenient low impedance point (such
as the error amp output) that enables accurate closed loop checking
of loop gain with a single floating voltage source - both on the lab
bench and on the circuit simulator.
By the way, as long as one isn't using the student version and doesn't
run out of nodes, making two copies in the same simulation file of the
circuit being checked for loop gain allows running with both voltage
and current drive simultaneously and may simplify probing the results.
> This *may* be applicable to other "Spices" as well.
I believe that this is a totally generic method, yes?
You obviously are a Pspice aficionado, Jim. There is a rather clever
way to force any circuit containing behavioral models, no matter how
non-linear, to always successfully reach an initial operating point
solution. It takes full advantage of Pspice's scheme of cutting back
all power source as a convergence seeking ploy together with a unity
voltage source as a reference node for taming the behavioral models.
Can you guess what it is? -- analog