I have spent some time searching this site for a good way to judge the stability of a power amp using LTspice, and there seems to be various techniques which seem to give different results. I think this is a popular question but usually atached to a specific circut, so I thought a new thread that was more general made sense.
I have seen people also use squarewave response or the slope of the open loop gain, but most use Bode plots, but they use different criteria for these plots: phase margins of closed loop gain, open loop gain, and loopgain (and the confusion starts with these names). In the Spice thread, J. Curl has posted the most comprehensive instructions and a big thanks should go out to him, but there is still confusion.
This is the way I understand it. Please correct me if I am wrong! First: most amps are stabilized using a Miller cap (or other integrater) in the cct.. This decreases the high Freq gain, which increases stability, but also increases the HF THD (less feedback). From this I deduce that one should use the the smallest Miller cap possible while maintaining stability.
Heres what I have seen: Squarewave response: If there is excesive ringing the amp is unstable, but what does excesive mean.
If the slope of the open loop response is to steep its unstable(this one dosnt make sense to me, its not how fast the gain hits zero but what the phase is doing, i know the two are directly related but to use this blanket statement with out showing the bode plot (phase) seems a stretch.
The 3 bode plot techniques are the same, phase margin at unity gain, but people use different plots. The only one that works properly is the loopgain plot. (this one takes the fedback into account). This uses the Middlebrook probe method JC has discribed in the Spice thread starting on post 864.
I have simmed these different Bode plots of a Blameless amp and got very different phase margins, has any one else tried this? I am I doing somethig wrong?
I have seen people also use squarewave response or the slope of the open loop gain, but most use Bode plots, but they use different criteria for these plots: phase margins of closed loop gain, open loop gain, and loopgain (and the confusion starts with these names). In the Spice thread, J. Curl has posted the most comprehensive instructions and a big thanks should go out to him, but there is still confusion.
This is the way I understand it. Please correct me if I am wrong! First: most amps are stabilized using a Miller cap (or other integrater) in the cct.. This decreases the high Freq gain, which increases stability, but also increases the HF THD (less feedback). From this I deduce that one should use the the smallest Miller cap possible while maintaining stability.
Heres what I have seen: Squarewave response: If there is excesive ringing the amp is unstable, but what does excesive mean.
If the slope of the open loop response is to steep its unstable(this one dosnt make sense to me, its not how fast the gain hits zero but what the phase is doing, i know the two are directly related but to use this blanket statement with out showing the bode plot (phase) seems a stretch.
The 3 bode plot techniques are the same, phase margin at unity gain, but people use different plots. The only one that works properly is the loopgain plot. (this one takes the fedback into account). This uses the Middlebrook probe method JC has discribed in the Spice thread starting on post 864.
I have simmed these different Bode plots of a Blameless amp and got very different phase margins, has any one else tried this? I am I doing somethig wrong?
cbdb said:
That would be Andy, our LTspice resident expert. JC needs no stinkin' spice, everything was already done 40 years ago, anyway.
Your are essentially correct in your descriptions; the correct stability analysis method is the loop gain phase margin at unity gain.
Post a schematic of your attempt to determine the loop gain phase margin and somebody will guide you through the LTspice specific process.
Try playing with LoopGain.asc and LoopGain2.asc in Educational folder of your LTSpice installation. Also, have a look at this thread http://www.diyaudio.com/forums/showthread.php?s=&postid=1814253#post1814253 and read about last 10 pages. There are two guys (if I remember correctly) asking questions about calculating open loop gain and phase. Andy C described it very well there.
My experience is that stability is one of the things that Spice predicts poorly. Amps that are unstable in simulation often turn out to be perfect in reality, and vice versa. This seems to be partly due to poor models, and partly the effect of stray reactance. You can add the latter to the sim, but the former is more difficult to fix.
Hi
look this link:
http://users.tpg.com.au/users/ldbutler/Waveforms.htm
there 3 bode plot:
1- Open loop gain: You can get bode plot the loop gain (Gain 0/1). Disconnecting the link feedback and connect the base of trasistor Q2 in GND (input - the differential pair )
You can get phase margin in open loop, we assume its open loop is 60dB and its closed loop gain 23dB, just go bode plot and see phase in 23dB we assume 100 degrees,(180-100), its phase margin is 80 degrees, more is not precise measure by this method.
2- Middlebrook: is the difference between open loop and closed -loop, you get the phase margin in 0dB (where it ends the difference between open loop and closed -loop), look the two bode plots you will understand.
3-Closed loop: to gain feedback on
Yes is correct, but low values requires quick transitor(low internal capacitance, Cu), may have problems with trasistores similarcbdb said:
Squarewave is another test, for example: may indicate local oscillation in output stage, that is not related the bode plot.cbdb said:
look this link:
http://users.tpg.com.au/users/ldbutler/Waveforms.htm
No, Middlebrook is more precise for this reason is used.cbdb said:
there 3 bode plot:
1- Open loop gain: You can get bode plot the loop gain (Gain 0/1). Disconnecting the link feedback and connect the base of trasistor Q2 in GND (input - the differential pair )
You can get phase margin in open loop, we assume its open loop is 60dB and its closed loop gain 23dB, just go bode plot and see phase in 23dB we assume 100 degrees,(180-100), its phase margin is 80 degrees, more is not precise measure by this method.
2- Middlebrook: is the difference between open loop and closed -loop, you get the phase margin in 0dB (where it ends the difference between open loop and closed -loop), look the two bode plots you will understand.
3-Closed loop: to gain feedback on
you should remove the input capacitors and zobel output, they are not part of the cycle feedback.cbdb said:
This is not correct. Spice adjusts the transistor HFE (Beta) for different collector currents and temperatures. Run a sim with a current source feeding the base of a transistor with a fixed voltage across the C-E. Then sweep the source and step the temp. and plot Ic/Iq you will see HFE curves (one for each temp step) that should look like the data sheets.
cbdb said:
I'm not really the LTspice resident expert. I think that honor belongs to jcx. His distortion residual calculator uses techniques that are way ahead of what I'm doing.
At any rate, for posting LTspice graphs and schematics, it helps to have a separate graphics application. I'd recommend the freeware IrfanView from Irfan Skiljan (www.irfanview.com). Here's the procedure. In LTspice, size your window to the final size you want your captured graphic to be. Then choose the "Tools, Copy Bitmap to Clipboard" menu item. Start up IrfanView. Do a Ctrl-V to paste the clipboard contents to the IrfanView window. Then do a "File, Save As" in IrfanView, and choose the ".PNG" extension. Don't use JPG, as this will become blurry. PNG works best with images that are "cartoon like" in the sense that they have lots of blocks of solid color (like schematics and graphs). Once you have a .PNG file, you can attach it to your post. If it's too big, you'll have to go back and recapture the graphic from a smaller window.
CBDB, <Enable your email button.> My apologies to others for going off-topic, though it may be useful information for anyone, using any program on a PC ...
With your schematic window open, hold down the Alt key and press the Print Scrn key. (This grabs the screen image and puts a copy of it into your PC's clipboard memory.) Next, launch Microsoft Paint. (Start> Programs> Accessories). With Paint running, hold down the Ctrl key and press the V key (This pastes the image into Paint. The schematic should appear in Paint.) Within Paint, just save the image as a GIF or PNG-24 file (don't use JPEG or BMP for this).
This forum expects the image to be less than 1000 pixels wide and under 100 kbytes. Use my email button if you need instructions for that part.
Hope that helps. <<Damn, Andyc beat me to it. And I agree with andyc about Irfanview>>
..Todd
With your schematic window open, hold down the Alt key and press the Print Scrn key. (This grabs the screen image and puts a copy of it into your PC's clipboard memory.) Next, launch Microsoft Paint. (Start> Programs> Accessories). With Paint running, hold down the Ctrl key and press the V key (This pastes the image into Paint. The schematic should appear in Paint.) Within Paint, just save the image as a GIF or PNG-24 file (don't use JPEG or BMP for this).
This forum expects the image to be less than 1000 pixels wide and under 100 kbytes. Use my email button if you need instructions for that part.
Hope that helps. <<Damn, Andyc beat me to it. And I agree with andyc about Irfanview>>
..Todd
"My experience is that stability is one of the things that Spice predicts poorly. Amps that are unstable in simulation often turn out to be perfect in reality, and vice versa. This seems to be partly due to poor models, and partly the effect of stray reactance. You can add the latter to the sim, but the former is more difficult to fix."
True - I have had similar expereinces. The value of Spice is that it allows you to tweak componenet values and see the effect, which is slightly different but can nevertheless be critically useful in understanding how and where to stabilize and amp.
True - I have had similar expereinces. The value of Spice is that it allows you to tweak componenet values and see the effect, which is slightly different but can nevertheless be critically useful in understanding how and where to stabilize and amp.
Bode plots are undoubtedly useful, but they generally only consider small-signal behavior and need to be supplemented by a look at step response, which also considers large-signal behavior. For DIYers who do not have access to a network analyzer, the combination of simulated Bode plots and bench tests with a square wave input voltage or load current can still tell you a lot about a circuit's performance.
The attached picture may help to translate what the scope shows in the time domain to what it means in the frequency domain.
The attached picture may help to translate what the scope shows in the time domain to what it means in the frequency domain.
- Status
- This old topic is closed. If you want to reopen this topic, contact a moderator using the "Report Post" button.