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.

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.

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.

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.

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.

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.

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.