The Cyber-Spy.Com Usenet Archive Feeds Directly
From The Open And Publicly Available Newsgroup
This Group And Thousands Of Others Are Available
On Most IS NNTP News Servers On Port 119.
Cyber-Spy.Com Is NOT Responsible For Any Topic,
Opinions Or Content Posted To This Or Any Other
Newsgroup. This Web Archive Of The Newsgroup And
Posts Are For Informational Purposes Only.
Reply-To: "fred bartoli"
From: "fred bartoli"
Subject: Re: SPICE and amp stability
Date: Wed, 20 Nov 2002 10:31:48 +0100
X-Newsreader: Microsoft Outlook Express 5.00.2314.1300
Organization: Guest of ProXad - France
NNTP-Posting-Date: 20 Nov 2002 10:28:56 MET
Kevin Aylward a écrit dans le message :
> Walter Harley wrote:
> > I have a simple 100mW audio amp circuit that, naively implemented, is
> > unstable at RF. The amp consists of an LM833 inverting stage with Av
> > = -4, followed by a push-pull emitter follower biased as class AB.
> > Feedback is taken from the output of the emitter follower.
> Typically, you might need an output stabilizing network for inductive
> loads (speakers). This is a series RC to ground at the output, and a
> parallel LR in series with the very output to the speaker. This puts a
> resistive load on the amp at HF, and disconnects the cables capacitance
> at HF.
> > I can stabilize the amp by putting a small-value capacitor between
> > the opamp output and the inverting input - basically taking the
> > emitter follower out of the loop at high frequencies. However,
> > unless I use a very tiny value, this causes substantial
> > intermodulation distortion as the emitter follower is not all that
> > linear without feedback. If I do use a tiny value, I'm concerned
> > that it won't be stable in real life.
> > Rather than just try cap values at random, I would like to really
> > understand what's going on. So, I'd like to model the phase response
> > and gain bandwidth of the system, and find a way to compensate the
> > circuit so that gain drops below unity by the frequency where there
> > is 180 degree phase shift. But I'm not sure how to do this, either
> > analytically or in PSpice, for four reasons that maybe y'all can help
> > me with:
> > 1) How do I figure out the phase response of the feedback network?
> > The only "capacitors" in the circuit are the input capacitance of the
> > opamp, which is not specified in the datasheets, and the various
> > parasitic capacitances, and whatever appears across the load
> > (probably cable capacitance). Do I just guess?
> You can guess the parasitic as a starter.
> > 2) To simulate the system and calculate a Bode plot, should I model
> > the parasitic capacitances in PSpice and then look at phase shift
> > between the circuit input and the inverting input of the opamp?
> No. The circuit input is the wrong place to measure loop gain
> > Or
> > is there some more correct way to determine the loop characteristics?
> 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:-). It is all set up to do this already. You can
> change the model attached to the opamp.
> In PSpice you might have to use an large inductor to brake the loop at
The easiest way the get the open loop gain is to stick an AC voltage source
somewhere in series with the loop (be sure there's no parallel path). Then
simply make the ratio of voltages at each end of this voltage source and you
have the loop gain.
Doing so, you're sure not to alter the loop gain what you can do with a loop
filter if you're not careful enough with the filter place in the loop
(relative input and output impedances of the stages at the break point) .
Also a zero DC voltage will always provide you with the right bias point for
the same reasons.
> > 3) Do the SPICE models for opamps accurately depict the bandwidth,
> > phase shift, and input capacitance in general? If not, which of
> > these parameters do I need to externally model?
> In generaly, they can be quite good.
> Kevin Aylward
> SuperSpice, a very affordable Mixed-Mode
> Windows Simulator with Schematic Capture,
> Waveform Display, FFT's and Filter Design.
Go Back To The Cyber-Spy.Com
Usenet Web Archive Index Of
The sci.electronics.design Newsgroup