Leach150 phase margin problem!!!

[mclarenpingu]

Hello Everybody!!
I have a problem of Leach 150
I have make a Leach150 power AMP and it is working fine, but in spice simulation
some problem confuse me very much!!
It is phase margin problem!!
I use Spice to simulate the Gain and Phase,
but I found the phase margin is not enough!, it almost 0 degree.
I simulate in transient it is very normal,
and the transient testing result use function generator that still no problem,
could I ignore the phase margin??, but in the text book, the PM at least is 35 drgree
or I am really too stupi that I simulate wrong??

please help me, thank you very much
have a nice day!!

[IMG]<a href="http://img185.imageshack.us/my.php?image=leachspicesd0.jpg" target="_blank"><img src="http://img185.imageshack.us/img185/3277/leachspicesd0.th.jpg" border="0" alt="Free Image Hosting at www.ImageShack.us" /></a>[/IMG]



The phase margin image is here!!

http://img528.imageshack.us/my.php?i...problemov3.jpg

I almost crazy, don't know what is wrong!!!

[gootee]

I am not familiar with your amp's circuit. But to find the phase margin, to judge the stability of a feedback system, you have to do it with the OPEN-loop gain and phase.

There are also ways to do it with the loop closed, such as the Tian method. You can look in the Files section of the LT-SPICE users' group, at http://tech.groups.yahoo.com/group/LTspice . There is a file you can download that gives the locations of all of the files. Then look for files called Loopgain3.asc and Loopgain2.asc . I use the second schematic in Loopgain3.asc . You can download Ltspice (aka SwitcherCad), to view the files, and then adapt them to whatever Spice you are using. LTspice can be downloaded here: http://ltspice.linear.com/software/swcadiii.exe .

Or, with "the simple method", you can insert an AC source just before a high-impedance input, such as the summing node for your feedback, with the source's + output toward the high-impedance node. If the AC source's + side is labeled In and the - side is labeled Out, then you can plot V(Out)/V(In). If the high-impedance node is really high-impedance, such as an opamp input, then the simple AC source method should be accurate-enough up to tens of MHz.

[mclarenpingu]

Hello Tom
Thanks your information
I give the AC signal in before the input filter,
this is AC in
and output I measure 2 point,
one is 3rd stage output (power AMP output)

another is 2nd stage output (voltage AMP output)

those result are almost the same,
this confuse me a lot

I also do the open-loop simulation, but the result is more bad
the phase reach -2xx degree

does leach150 itself have low phase margin naturally???

thanks a lot !!!

have a nice day!!!

[mclarenpingu]

Hello My Lord!!

I upload some PIC in the imageshack, because my first post some pic cannot see

Pic1: it is my schematic, it was a little modify from original Leach150
the source is one Chinese audio DIY site http://www.diyzone.net/index.php

http://img134.imageshack.us/my.php?image=dzleachmm1.jpg

Pic2: it is my spice schematic

http://img182.imageshack.us/my.php?i...chspicemd9.jpg

Gain and Phase simluation result

http://img518.imageshack.us/my.php?i...hasesimsb7.jpg

It is so stranger, please help me!! thanks very much!!

[pooge]

Originally posted by mclarenpingu
Hello Tom
Thanks your information
I give the AC signal in before the input filter,
this is AC in
and output I measure 2 point,
one is 3rd stage output (power AMP output)

I think you should input AFTER the input filter. The input filter will cause a phase change related to its cutoff frequency, which is much lower than the amplifier bandwidth, per se, and is outside the feedback loop.

[gootee]

Originally posted by mclarenpingu
Hello Tom
Thanks your information
I give the AC signal in before the input filter,
this is AC in
and output I measure 2 point,
one is 3rd stage output (power AMP output)

another is 2nd stage output (voltage AMP output)

those result are almost the same,
this confuse me a lot

I also do the open-loop simulation, but the result is more bad
the phase reach -2xx degree

does leach150 itself have low phase margin naturally???

thanks a lot !!!

have a nice day!!!

Using your normal input point, before the input filter, with the system running closed-loop, will _NOT_ work, for phase-margin stability analysis. No way. Don't bother. You're totally wasting your time. (Is that clear-enough?! :-)

Perhaps you could post the spice schematic for your open-loop analysis, and the resulting gain and phase plot. THEN maybe someone can help you.

[gootee]

I just remembered that I already posted an example of the Tian method, with LTspice, here:

http://www.diyaudio.com/forums/showt...t=#post1298611

That post does not include any stability results, but DOES include a JPEG of the circuit schematic, showing the Tian stability "probe" inserted into the closed-loop system (AND a downloadable ZIP file containing the LTspice simulation files).

In case you don't want to download LTspice, you can just look at that schematic, make your own, and get the details correct by copying and pasting into your spice schematic, from the following:

If you insert a series AC voltage source, named

Vi

as shown in the schematic, with AC amplitude

{u(-prb)}

and, after that, an AC current source from ground, named

li

(i.e. L and I), with AC amplitude

{u(prb)}

and label the node where they join with the name

x

and run an AC Analysis and step the prb parameter from -1 to 1, with the spice directive:

.step param prb list -1 1 ; set prb=0 to turn off probe

using the AC Analysis directive:

.ac dec 30 .001 10Meg

then you can plot the open-loop gain and phase by plotting the following expression:

1/(1-1/(2*(I(Vi)@1*V(x)@2-V(x)@1*I(Vi)@2)+V(x)@1+I(Vi)@2))

I always grounded the signal-input node, when running the above for stability analysis.

[mclarenpingu]

Hello gootee
Thanks your great help
I think I might be wrong and I see the Phase margin to the dB axis
because I am simulate in midnight.....feel so tired............
sorry

Today I do some simulate I feel input filter seem no the root cause
I will follow you instruction and so the simulation
and I will post the result ASAP

thanks a lot!!!!!

[mclarenpingu]

Hello
Thanks master Gootee
I have download LTspice
it have many example for simulation, I think it is a good program,
Although I use OrCad P-spice to simulation
but LTspice is a very good utility for research!!!

thanks very much!!

[AndrewT]

Hi,
that schematic looks like a Leach Low Tim but with a CCS added to source the LTP tails.