Hello,

Under
http://groups.yahoo.com/group/LTspice/files/Examples/Educational/LoopG
ain_Probe/, I have uploaded an extended version of the LoopGain
example that comes with LTspice. The voltage and current sources for
simulating the loop gain are conveniently placed inside a subcircuit,
which plays the role of a "loop gain probe". These sources are
controlled by a variable and are activated one at a time by a .step
command, so that it is not necessary to duplicate the circuit. The
step selection operator @ is used to compute the loop gain from the
simulation results. In order to simulate the "normal" closed-loop
gain of the circuit, both sources in the probe subcircuit can be
turned off by setting the control variable to zero.

The example also features a generalized version of Middlebrook's
formula that was developed by Michael Tian and takes backward loop
transmission into account. The result of this formula is independent
of the direction in which the probe subcircuit is inserted. In a loop
with no backward transmission, the result of Tian's formula is
identical to that of Middlebrook's formula. Tian's formula is used by
the stability analysis of the Spectre circuit simulator from Cadence
Design Systems.

By the way, has anyone found a way to calculate phase margin and gain
margin in LTspice, so that one does not have to use the cursors each
time to read the values?

Best regards,

Frank

--- In LTspice@..., "Frank Wiedmann"
<frank.wiedmann@w...> wrote:

Hello Frank,
thanks for these circuit files. First I had problems to test your
circuits until I realized that I have to switch on the storage of
subcircuit currents and voltages.

Control Panel->Save Defaults
x Save Device Currents
x Save Subcircuit Node Voltage
x Save Subcircuit Device Current

Please add a comemnt to your schematic about this.

My understanding of this Middlebrook method is that it should be
possible to calculate the open loop gain of an embedded amplifier.

Now my results:
I used your example but replaced the amps by LT1013. I also changed
the load resistor to 100kOhm and the feedback resistor to 10kOhm.
An additional capacitor of 1pF/100pF have been added at the -input to
test whether this method is insensitive to that or not.

I then added the "classical" open loop gain test circuit.

When I now compare the result, the open loop gain of your
configuration is 20dB off (it's exactly Rfeedback/Rsource) at low
frequency.
Why this?
What have I understand wrong about Middlebrook's method?

I also realized that the result differs at high frequency if I change
the capacitors CTx at the -input to 100pF.

Please help me to understand what's going wrong.

I added my files to your folder. We can move my files later to
another folder if you want that.

Best Regards,
Helmut

http://groups.yahoo.com/group/LTspice/files/Examples/Educational/LoopG

ain_Probe/, I have uploaded an extended version of the LoopGain
example that comes with LTspice. The voltage and current sources

for

simulating the loop gain are conveniently placed inside a

subcircuit,

which plays the role of a "loop gain probe". These sources are
controlled by a variable and are activated one at a time by a .step
command, so that it is not necessary to duplicate the circuit. The
step selection operator @ is used to compute the loop gain from the
simulation results. In order to simulate the "normal" closed-loop
gain of the circuit, both sources in the probe subcircuit can be
turned off by setting the control variable to zero.

The example also features a generalized version of Middlebrook's
formula that was developed by Michael Tian and takes backward loop
transmission into account. The result of this formula is

independent

of the direction in which the probe subcircuit is inserted. In a

loop

with no backward transmission, the result of Tian's formula is
identical to that of Middlebrook's formula. Tian's formula is used

by

the stability analysis of the Spectre circuit simulator from

Cadence

Design Systems.

By the way, has anyone found a way to calculate phase margin and

gain

margin in LTspice, so that one does not have to use the cursors

each

time to read the values?

Best regards,

Frank

--- In LTspice@..., Frank Wiedmann wrote:

Hello, Under

http://groups.yahoo.com/group/LTspice/files/Examples/Educational/LoopG
ain_Probe/

I have uploaded an extended version of the LoopGain example
that comes with LTspice. The voltage and current sources for
simulating the loop gain are conveniently placed inside a sub
circuit, which plays the role of a "loop gain probe". These
sources are controlled by a variable and are activated one at a
time by a .step command, so that it is not necessary to duplicate
the circuit. The step selection operator @ is used to compute
the loop gain from the simulation results. In order to simulate
the "normal" closed-loop gain of the circuit, both sources in the
probe subcircuit can be turned off by setting the control variable
to zero.

Very impressive use of waveform math with hierarchical subcircuits.
Did you learn about the @ operator from reading this Yahoo Group,
from the recent changes to the help file, or from prior experience
with another simulator?

The example also features a generalized version of Middlebrook's
formula that was developed by Michael Tian and takes backward loop
transmission into account. The result of this formula is independent
of the direction in which the probe subcircuit is inserted. In a
loop with no backward transmission, the result of Tian's formula is
identical to that of Middlebrook's formula. Tian's formula is used
by the stability analysis of the Spectre circuit simulator from
Cadence Design Systems.

Thanks for the very nice contribution to the LTspice community. I
checked the technique with a three stage, equal element RC low pass
network feeding back to a VCVS with gain set to 30 such that it just
barely oscillates in a transient simulation. The probe may be
inserted with either orientation at the VCVS or in the middle of the
RC network without effecting the transient results. Yet it always
yields the same, correct ac loop gain simulation results. As a
matter of taste, I changed the polarity of the math expression to
make the phase go to 0 rather than -180 at the point of oscillation.

By the way, has anyone found a way to calculate phase margin and
gain margin in LTspice, so that one does not have to use the
cursors each time to read the values?

The cursor method seems very easy and convenient. How and in what
other format would you like LTspice to do this? Also, automated
methods tend to have problems with conditionally stable systems, in
which case a visual inspection would be required anyway.

Regards -- analog(spiceman)

--- In LTspice@..., "Helmut Sennewald"
<helmutsennewald@y...> wrote:

--- In LTspice@..., "Frank Wiedmann"
<frank.wiedmann@w...> wrote:

Hello Frank,
thanks for these circuit files. First I had problems to test your
circuits until I realized that I have to switch on the storage of
subcircuit currents and voltages.

Control Panel->Save Defaults
x Save Device Currents
x Save Subcircuit Node Voltage
x Save Subcircuit Device Current

Please add a comemnt to your schematic about this.

Done.

My understanding of this Middlebrook method is that it should be
possible to calculate the open loop gain of an embedded amplifier.

Now my results:
I used your example but replaced the amps by LT1013. I also changed
the load resistor to 100kOhm and the feedback resistor to 10kOhm.
An additional capacitor of 1pF/100pF have been added at the -input

to

test whether this method is insensitive to that or not.

I then added the "classical" open loop gain test circuit.

When I now compare the result, the open loop gain of your
configuration is 20dB off (it's exactly Rfeedback/Rsource) at low
frequency.
Why this?
What have I understand wrong about Middlebrook's method?

I also realized that the result differs at high frequency if I

change

the capacitors CTx at the -input to 100pF.

Please help me to understand what's going wrong.

Opening the loop for simulating loop gain is generally not
recommended because of the difficulties in getting the correct dc
operating point and the correct impedances.

However, in this particular example it works actually quite well. Of
course, you have to go all the way around the loop in order to get
the loop gain. So, if you measure the voltage at CT4/R13, you will
get a result that is very close to that of the loop gain formulas.

Best regards,

Frank

--- In LTspice@..., "analogspiceman"
<analogspiceman@y...> wrote:

Very impressive use of waveform math with hierarchical subcircuits.
Did you learn about the @ operator from reading this Yahoo Group,
from the recent changes to the help file, or from prior experience
with another simulator?

From the changelog file, in fact, in connection with prior experience
with other simulators.

By the way, has anyone found a way to calculate phase margin and
gain margin in LTspice, so that one does not have to use the
cursors each time to read the values?

The cursor method seems very easy and convenient. How and in what
other format would you like LTspice to do this? Also, automated
methods tend to have problems with conditionally stable systems, in
which case a visual inspection would be required anyway.

Well, I am a lazy person, so I would like to have a function that
returns the numeric value without me having to move the cursors
around. Of course, I would still look at the loop gain curve in order
to see if anything strange happens.

Best regards,

Frank

--- In LTspice@..., Frank Wiedmann wrote:

--- In LTspice@..., analogspiceman wrote:

--- In LTspice@..., Frank Wiedmann wrote:

Next to your original files I have uploaded a zip file that
includes my test circuit with the three stage, equal element RC
low pass network of which I wrote in my prior post. I also took
the liberty of making a few "improvements" to your subcircuit to
make it easier to use.

Very impressive use of waveform math with hierarchical
subcircuits. Did you learn about the @ operator from reading
this Yahoo Group, from the recent changes to the help file, or
from prior experience with another simulator?

From the changelog file, in fact, in connection with prior
experience with other simulators.

Although LTspice's help file is very good, it does not cover all
of the useful features built in to LTspice. I've made a kind of
LTspice help file crib sheet that fills in most of the blanks with
regard to LTspice's math functions for B-sources and waveforms.
It is here in the files section under "adventures with analog" as
Waveform_Arithmetic_&_B-sources.pdf. You might give it a look see.

By the way, has anyone found a way to calculate phase margin
and gain margin in LTspice, so that one does not have to use
the cursors each time to read the values?

The cursor method seems very easy and convenient. How and in
what other format would you like LTspice to do this? Also,
automated methods tend to have problems with conditionally
stable systems, in which case a visual inspection would be
required anyway.

Well, I am a lazy person, so I would like to have a function
that returns the numeric value without me having to move the
cursors around. Of course, I would still look at the loop gain
curve in order to see if anything strange happens.

Right now there is no tool to automatically present you with
numeric gain and phase margins. I suppose it could be added to
the data in the output (log) file, or be made available in a
message window similar to the average/RMS calculation, but it
still would require exercising the mouse about as much as the
cursor method. Now I am curious about what you had in mind.
If you could relieve that curiosity by describing precisely
how you imagined this feature might be implemented, I would be
appreciative. -- analog(spiceman)

--- In LTspice@..., "Frank Wiedmann"
<frank_wiedmann@y...> wrote:

--- In LTspice@..., "Helmut Sennewald"
<helmutsennewald@y...> wrote:

--- In LTspice@..., "Frank Wiedmann"
<frank.wiedmann@w...> wrote:

...
Please help me to understand what's going wrong.

Opening the loop for simulating loop gain is generally not
recommended because of the difficulties in getting the correct dc
operating point and the correct impedances.

However, in this particular example it works actually quite well.

Of

course, you have to go all the way around the loop in order to get
the loop gain. So, if you measure the voltage at CT4/R13, you will
get a result that is very close to that of the loop gain formulas.

Hello Frank and "analogspiceman",
I think I have understood it now. The Middlebrook method calculates
the "open" loop gain of the actual configuration. This is not
necessarily the open loop gain of the opamp which is shown in the
datasheet.

The open loop gain from this method can be used to determine the
stability of a circuit. It is stable, if the phase shift is less than
180degree at the gain point 0dB.

I tested the circuit from "analogspiceman" too. It's very impressive
that the probe can be moved around the circuit and we still get the
same result for the open loop gain.

Thanks to you both for presenting these methods with LTSPICE.

I will now remove my files from this folder, because they add no
value to the presentation.

Best Regards,
Helmut

--- In LTspice@..., "analogspiceman"
<analogspiceman@y...> wrote:

--- In LTspice@..., Frank Wiedmann wrote:

--- In LTspice@..., analogspiceman wrote:

--- In LTspice@..., Frank Wiedmann wrote:

Next to your original files I have uploaded a zip file that
includes my test circuit with the three stage, equal element RC
low pass network of which I wrote in my prior post. I also took
the liberty of making a few "improvements" to your subcircuit to
make it easier to use.

Thank you for your effort. In order to avoid any possible confusion,
you might want to add a short remark regarding the differences
between our approaches: The function of the values 1 and -1 of the
control variable has been exchanged and the loop gain according to
your formula is the loop gain of my formula multiplied by -1 (meaning
that the phases differ by 180 degrees).

Both sign conventions for the loop gain are actually being used by
different people. Yours is probably more logical from a mathematical
point of view and it is in fact the one that Tian uses in his
article. My definition is often used by circuit designers because
Bode used this sign convention for his "return ratio" in his classic
book "Network Analysis and Feedback Amplifier Design" (he did not use
the term "loop gain"). With this sign convention, the phase of the
loop gain is 0 degrees at low frequencies for most practical
circuits, a fact that many designers find convenient.

By the way, has anyone found a way to calculate phase margin
and gain margin in LTspice, so that one does not have to use
the cursors each time to read the values?

The cursor method seems very easy and convenient. How and in
what other format would you like LTspice to do this? Also,
automated methods tend to have problems with conditionally
stable systems, in which case a visual inspection would be
required anyway.

Well, I am a lazy person, so I would like to have a function
that returns the numeric value without me having to move the
cursors around. Of course, I would still look at the loop gain
curve in order to see if anything strange happens.

Right now there is no tool to automatically present you with
numeric gain and phase margins. I suppose it could be added to
the data in the output (log) file, or be made available in a
message window similar to the average/RMS calculation, but it
still would require exercising the mouse about as much as the
cursor method. Now I am curious about what you had in mind.
If you could relieve that curiosity by describing precisely
how you imagined this feature might be implemented, I would be
appreciative. -- analog(spiceman)

Well, to make this a more general feature, I could imagine a function
that returns the x-value of the zero crossing of a curve and a second
function that returns the y-value of a curve for a given x-value. By
inserting the first function into the second, one could form
expressions for phase margin and gain margin. Another possible
application of the first function would be finding the 3-dB frequency
of a filter. Additional functions detecting e.g. the maximum or
minimum of a curve might also be useful in this context.

Best regards,

Frank

http://groups.yahoo.com/group/LTspice/files/Examples/Educational/LoopG
ain_Probe/, I have uploaded an extended version of the LoopGain
example that comes with LTspice. The voltage and current sources for
simulating the loop gain are conveniently placed inside a subcircuit,

Thank you for this great subcircuit & example. I am trying to figure
out how to arrive at the equation that is plotted in LTSpice from the
equation in Tian's paper, "Striving for Small-Signal Stability".
(Equation 30)

I am still trying to understand this technique. Can someone show me
the relationship between these two equations?

LTSpice plot:
1/(1/(2*(I(V:lp:inj)@1*V(lp:probe)@2-V(lp:probe)@1*I(V:lp:inj)@2)+V(lp:probe)@1+I(V:lp:inj)@2)-1)

Tian Equation (30)
T= [2(AD-BC)-A+D] / [2(BC-AD)+A-D+1]

--- In LTspice@..., "xrinlar" <xrinlar@y...> wrote:

http://groups.yahoo.com/group/LTspice/files/Examples/Educational/LoopG

ain_Probe/, I have uploaded an extended version of the LoopGain
example that comes with LTspice. The voltage and current sources

for

simulating the loop gain are conveniently placed inside a

subcircuit,

Thank you for this great subcircuit & example. I am trying to

figure

out how to arrive at the equation that is plotted in LTSpice from

the

equation in Tian's paper, "Striving for Small-Signal Stability".
(Equation 30)

I am still trying to understand this technique. Can someone show me
the relationship between these two equations?

LTSpice plot:
1/(1/(2*(I(V:lp:inj)@1*V(lp:probe)@2-V(lp:probe)@1*I(V:lp:inj)@2)+V

(lp:probe)@1+I(V:lp:inj)@2)-1)

Tian Equation (30)
T= [2(AD-BC)-A+D] / [2(BC-AD)+A-D+1]

It's actually pretty straightforward algebra. First of all, I divide
numerator and denominator of the expression by its numerator and
rearrange the terms of the new denominator:

T = [2(AD-BC)-A+D] / [2(BC-AD)+A-D+1]
T = 1 / {-1 + 1 / [2(AD-BC)-A+D]}
T = 1 / {1 / [2(AD-BC)-A+D] - 1}

Now, we have to obtain the values for A, B, C, and D from simulation.
For the first step (@1) of the simulation, we have Vinj=1 and Iinj=0;
for the second step (@2), we have Iinj=1 and Vinj=0. You should also
notice that a positive current through Vinj is defined in the
opposite direction of If in the article because in Spice, a current
is defined as positive when it flows into the positive terminal of a
component. So, we have If = -I(V:lp:inj) as the negative current
through Vinj and Ve = V(lp:probe) as the voltage at the node
named "probe". Now, it is easy to write down the expressions for the
terms A, B, C, and D:

A = -I(V:lp:inj)@2
B = -I(V:lp:inj)@1
C = V(lp:probe)@2
D = V(lp:probe)@1

In order to make the expression look a little more elegant, I finally
introduce A' = -A and B' = -B and rearrange the terms a little bit:

T = 1 / {1 / [2(B'C-DA')+D+A'] - 1}

When you insert the expressions from above, you will get exactly the
formula that I am using in my example.

Best regards,

Frank

In order to make the expression look a little more elegant, I finally
introduce A' = -A and B' = -B and rearrange the terms a little bit:

T = 1 / {1 / [2(B'C-DA')+D+A'] - 1}

When you insert the expressions from above, you will get exactly the
formula that I am using in my example.

Best regards,

Frank

Great explanation, great circuit. Thank you.

Could you help me figure out, why the Middlebrook loop gain corresponds to the quantity 1/(V(Xlp:probe)@1+I(Xlp:Vprobe)@2)-1?
Many thanks
brette

--- In LTspice@..., "brette_83" <benedikt.bretthauer@...> wrote:

Could you help me figure out, why the Middlebrook loop gain corresponds to the quantity 1/(V(Xlp:probe)@1+I(Xlp:Vprobe)@2)-1?
Many thanks
brette

I will use the notation from http://www.spectrum-soft.com/news/spring97/loopgain.shtm for my explanation. For my formula, I am using the fact that the amplitude of my voltage and current sources is 1 when they are active, so that
Vf + Vi = 1 and
If + Ii = 1.
(The ground node is the negative terminal for Vi but the positive terminal for Vf, the drawing is not clear in this respect.)

Using these two equations, we get
Gv + 1 = Vf/Vi + 1 = (Vf + Vi)/Vi = 1/Vi and
Gi + 1 = If/Ii + 1 = (If + Ii)/Ii = 1/Ii.

With these results, we can easily calculate the loop gain:
1/(G + 1) = 1/(Gv + 1) + 1/(Gi + 1) = Vi + Ii
G + 1 = 1/(Vi + Ii)
G = 1/(Vi + Ii) - 1.

Best regards,

Frank

On Thu, Oct 31, 2024 at 12:50 AM, <m.compadre.t@...> wrote:

Hi,

Thanks for the great explanations.
I have a question. In the file, on the left hand side, there are two circuits
that use Middlebrook's approach. I've also tested the circuit with the classic
method of injecting an AC source from ground, and breaking the loop with an
L-C network. The results are exactly the same as the given examples.
However, when I use the Tian probe equation, the Bode plot looks completely
different. Has anyone encountered the same issue? I believe I've followed all
the instructions in the file, which are also contained within this thread.

I've uploaded the files in the following folder:
https://groups.io/g/LTspice/files/Temp/LoopGain_Probe_MC

Thank you!
Marcos

I suggest that you take a look at https://groups.io/g/LTspice/topic/50255277#msg108476

Best regards,
Frank

On Wed, Nov 6, 2024 at 03:10 PM, CEHymowitz wrote:

You might look into NISM. This is likely a much better and more accurate way
to assess loop stability (via output impedance).

This might be true for measurements in the lab, but I doubt that it is also true for SPICE simulations.

Best regards,
Frank