The Designer's Guide Community Forum

The Designer's Guide Community Forum
https://designers-guide.org/forum/YaBB.pl
Simulators >> Circuit Simulators >> stability analysis from ADE
https://designers-guide.org/forum/YaBB.pl?num=1220974790

Message started by Dipankar on Sep 9^th, 2008, 8:39am

Title: stability analysis from ADE
Post by Dipankar on Sep 9^th, 2008, 8:39am

Dear All,

I was trying stb analysis from ADE to characterize open loop dc gain ( in this case loop gain in unity feedback) , phase margin, ugbw of a 2 stage opamp .

The loopgain maxima as measured from stb analysis is matching exactly with dcgain measured from traditional openloop simulation tb. But pm reported by stb is less than what I get from my traditional testbench. Looks like the 2nd pole in case of stb analysis frequency response is occurring a bit earlier than that of traditional TB freq. response.

My traditional TB : opamp in non-inverting mode with rc feedback (lowpass filter with fc~1e-9 Hz) .

stb analysis TB: opamp in non-inverting mode with unity feedback (a dummy vdc in the loop)

Can anybody help me understand the case ? Which result I can rely upon ?

with regs.,
Dipankar.

Title: Re: stability analysis from ADE
Post by Tlaloc on Sep 9^th, 2008, 9:47am

I personally would believe STB analysis. The problem with the older methods of finding the transfer function involved a number of assumptions that discounted non-idealities. With a giant RC in the feedback (or LC) you have created a pole-zero pair at very low frequencies. This also isolates the real loading created by your input capacitance. It also isolates the feed-forward transmission (going the wrong way) through your feedback path. It does, though, approximate the real transfer function by providing something close to the voltage loop gain (see below).

Better methods include methods proposed by Middlebrook in 1975 that requires you to look at both the voltage (Tv) and current (Tc) transfer functions. This would generally require you to run two different simulations or have two copies of your amp in one simulation. Then, the combined transfer function is 1/(1+T)=1/(1+Tv)+1/(1+Tc). For low frequencies, the Tv term almost always dominates (which is why people continue to use the same method as you did), but at high frequencies, Tc can come into play.

The main problem with the previous approach is that it assumes a zero reverse loop gain. Since then, there has been some advances in the mathematics to account for all possible transmission paths. Middlebrook has published one method using the Dissection Theorem, but the Spectre stb analysis uses a alternate method. The math behind it shows that the answer should be much closer to reality, especially at high frequencies where the non-idealities dominate, than previous methods.

In short, I would trust stb, especially since it is providing the more conservative answer.

Title: Re: stability analysis from ADE
Post by Dipankar on Sep 9^th, 2008, 10:28am

Thanks .

Title: Re: stability analysis from ADE
Post by Frank Wiedmann on Sep 9^th, 2008, 11:49pm

The method used by the stb analysis of Spectre is described in http://www.kenkundert.com/docs/cd2001-01.pdf. Additional information about loop gain simulation can be found on my webpage http://www.geocities.com/frank_wiedmann/loopgain.html.

Title: Re: stability analysis from ADE
Post by nobody on Sep 11^th, 2008, 8:34pm

Hello, Frank

You use LTspice to simulate the loop gain. I was wondering if we can use the way you did in LTspice by using Hspice.

Title: Re: stability analysis from ADE
Post by Frank Wiedmann on Sep 12^th, 2008, 12:13am

I have never worked with Hspice, so I do not know if it is possible there to combine the results for different values of a sweep variable in an expression. In case this should not be possible, you can still use several copies of your circuit in a single schematic. Each circuit would then have to be configured corresponding to one of the values of the sweep variable in LTspice.

Title: Re: stability analysis from ADE
Post by Tlaloc on Sep 12^th, 2008, 9:49am

There is not a way to directly post-process values from multiple sweeps in HSpice. The .MEAS statement is limited to the current simulation only. You will have to use some other tool to do that, e.g. a scripting program or Matlab.

Title: Re: stability analysis from ADE
Post by nobody on Sep 14^th, 2008, 2:00am

Hello, Tlaloc
My problem is probably what you talked about. I have no idea how to get a math calculation via HSPICE from mulitple sweeps because I need to know the result from the exact run like 1st or 2nd sweep. For LTspice, it is convient and powerful to specify what run I want by using @ operator . Thank you, all.

Title: Re: stability analysis from ADE
Post by nobody on Sep 17^th, 2008, 1:16am

Hello, Frank

I tried your way in Hspice and simulated a simple common source samplifier with shunt-shunt feedback like the one in "Striving for Small-Signal Stability". The loop-gain looks good. However, the loop-gain looks wrong if I insert the "loog gain probe" in the opposite direction like you did in your example. Plus, the loop-gain looks the same if I turn on or off the local return loops by doing the same setting in the article and the result is supposed to be different. That is strange. I wish I will figure that out soon.

Title: Re: stability analysis from ADE
Post by Frank Wiedmann on Sep 17^th, 2008, 4:50am

I would suggest that you verify your formulas, especially the signs, and also the orientation of all the sources in the loop gain probe. There is probably an error in your formula concerning a term that is small for one direction but large for the opposite direction.

Title: Re: stability analysis from ADE
Post by nobody on Sep 18^th, 2008, 12:36am

Hello, Frank

Thanks for your reply. I use the equation T = 1 / {1 / [2(B'C-DA')+D+A'] - 1} in your example and upload a figure to how I test the circuit. I will try to verify things you talked. Thanks again

Title: Re: stability analysis from ADE
Post by Frank Wiedmann on Sep 18^th, 2008, 11:09am

I did not find an error in your drawing. To help you debug your setup in Hspice, you could simulate the same circuit with LTspice using my original loop gain probe. You could first verify that you get the same result for both orientations of the probe. After that, you could plot the results for parts of the expression for the loop gain in both Hspice and LTspice until you see where the difference comes from.

Title: Re: stability analysis from ADE
Post by wave on Sep 18^th, 2008, 12:47pm

If you are using Hspice, I believe they have the equivalent of STB.
Look in your manual.

Eldo also has a single ended version of STB. They didn't have a diff'l setup last I knew.

~Wave

Title: Re: stability analysis from ADE
Post by Tlaloc on Sep 18^th, 2008, 12:58pm

I personally have never seen a stb equivalent in HSPICE. The latest version that I used was 2006, and I didn't see it there. I haven't looked closely enough at Eldo to say one way or the other.

Title: Re: stability analysis from ADE
Post by nobody on Sep 18^th, 2008, 5:08pm

Thanks, Frank

I will try ways to verify. I will go with Tlaloc because I have never seen the equivalent of STB or magic "iprobe" in Hspice.

Title: Re: stability analysis from ADE
Post by Frank Wiedmann on Sep 19^th, 2008, 12:08am

Tlaloc wrote on Sep 18^th, 2008, 12:58pm:

I personally have never seen a stb equivalent in HSPICE. The latest version that I used was 2006, and I didn't see it there. I haven't looked closely enough at Eldo to say one way or the other.

Regarding Eldo, I found http://www.edaboard.com/ftopic265486.html. It seems to use Middlebrook's old method from 1975 that was developed without taking into account backward transmission.

Title: Re: stability analysis from ADE
Post by imd1 on Sep 19^th, 2008, 5:43am

Frank Wiedmann wrote on Sep 19^th, 2008, 12:08am:

Tlaloc wrote on Sep 18^th, 2008, 12:58pm:

I personally have never seen a stb equivalent in HSPICE. The latest version that I used was 2006, and I didn't see it there. I haven't looked closely enough at Eldo to say one way or the other.

Regarding Eldo, I found http://www.edaboard.com/ftopic265486.html. It seems to use Middlebrook's old method from 1975 that was developed without taking into account backward transmission.

Why do you think that eldo is using the old method ? I am curious how to go about testing for this.

So, AFAWK Spectre (and LTspice!) are the only simulators that support the (correct?) loop gain test fixture ?

Title: Re: stability analysis from ADE
Post by Frank Wiedmann on Sep 19^th, 2008, 11:08am

imd1 wrote on Sep 19^th, 2008, 5:43am:

Why do you think that eldo is using the old method ? I am curious how to go about testing for this.

I concluded this from one of the messages in http://www.edaboard.com/ftopic265486.html :

Code:

* .lstb This command improves the analysis of circuit stability.
* The .LSTB command measures the loop gain by successive injection (Middlebrook
* Technique). A zero voltage source is placed in series in the loop: the first pin of the voltage loop
* must be connected to the loop input, the other pin to the loop output.

It mentions Middlebrook but not his General Feedback Theorem.

Quote:

So, AFAWK Spectre (and LTspice!) are the only simulators that support the (correct?) loop gain test fixture ?

The only simulator I know which has Tian's method directly built in is Spectre. In LTspice, I have implemented it by using some ideal sources together with a parameter sweep and an expression that calculates the loop gain from the simulation results. It should be possible to implement Tian's method in a similar way in most other Spice simulators.

The question regarding the correct loop gain is a bit more difficult to answer. From a usability standpoint, I like Tian's method best because of its symmetry. With respect to formal correctness, Middlebrook's General Feedback Theorem probably has the better arguments on its side. This question is somewhat academic, however, because for practical circuits, the results of all three methods discussed here are usually very close to each other. They also will all tell you correctly if the circuit is stable or not (see my webpage http://www.geocities.com/frank_wiedmann/loopgain.html for details).

Title: Re: stability analysis from ADE
Post by nobody on Sep 25^th, 2008, 3:02am

Hello, Frank

Your method is right and I made a trival mistake. The place where you want to put the magic "probe" does not matter, which is verified in your example. I did the same thing and get the same result. However, I get a slight change in the result like GBW by using the stb analysis. DC gaim and phase margin are same. DC operating parameters like Vgs, Vds, gm, gmb, and cdtot are same.
GBW(Tian's method)=144MHz GBW(STB)=255MHz
I was wondering if you have any idea why there is a change in GBW.

Title: Re: stability analysis from ADE
Post by Frank Wiedmann on Sep 25^th, 2008, 5:40am

I have no idea where the difference comes from. Spectre's stb analysis uses Tian's method and you should get exactly the same result if your circuit and your device models are the same. Maybe there is another error in your setup?

Title: Re: stability analysis from ADE
Post by nobody on Apr 9^th, 2009, 7:46pm

Hello, Frank

I read the website you said. To get the loop gain of differential CKT, I have to add a "balun". I went to your website but I can not find examples about the simulation loop gain of differential CKT. I was wondering if you can provide me some suggestions or examples to simuate the loop gain of differential CKT.
Thanks.

Title: Re: stability analysis from ADE
Post by nobody on Apr 10^th, 2009, 5:42am

Hello, Frank

I think I kind of understand what you talked in your website and just try to draw a photo for verification. If the method in the photo is right, I can use the same way to simulate the common mode loop. All I have to do is put a probe in the common mode path.
Thanks.