Dear colleagues!

I deal with SPICE models for SOI MOSFETs. Self-heating effect is one of the most important problems for the designer because it's difficult to obtain the values of cth0 and rth0 parameters.

My objective is to study or develop the methodology for the extraction procedure for these parameters.

Unfortunately I actually don't know how this effect is modeled by simulator. BSIMSOI model has a separate pin "t" for the "intrinsic" temperature, but how is this information used by simulator?

I found the following formula:
P=ΔT/rth + cth*δ(ΔT)/δt,
where ΔT is the difference between "intrinsic" temperature and ambient, t is time, P is the power dissipation.

How this "P" is used for recalculation of Ids?

In another words, it's unclear for me how a simulator solve the equations for SHE. Let's consider the simple example:
1) Ids is calculated.
2) P=Ids*Vds.
3) A simulator "knows" rth and cth.
4) As far as I understand the simulation process, Ids is to be recalculated to obtain a negative output resistance (static IV). The first question is how to recalculate Ids? The second is the following: does "P" is also recalculated after the Ids changing? So, when will the recalculation process stop?

Thanks in advance.

Dear Sheldon!

There is unfortunately no answers for my questions in the manual... Let me explain. If we look at the Fig. 5.1 (page 34) we would see that there is power dissipation (P=Ids*Vds) and thermal resistance and capacitance, but how is decrease of the drain current simulated? There is only few words about "T" terminal:
"The T node is treated as a voltage node and is connected to ground through a thermal resistance Rth and a thermal capacitance Cth"

No any words about thermal coupling between devices, no information about Ids recalculation... It is probably evident for the community, but I really don't understand the simulation process...

... and, during the model evaluation for BSIMSOI, many of the parameters of the device are re-adjusted for the self-heating temperature, and Ids (etc) is computed using the re-adjusted parameters.

(BSIM3/BSIM4 etc adjust parameters once at the beginning of the simulation for the ambient temperature.)

In BSIMSOI, the T node acts just like a regular electrical node: the "voltage" on that node is solved for, just like all the other voltages in the circuit (Spice's modified nodal analysis).

The T node has a "current source" (Ids*Vds) and a resistor (using your case Cth=0), and Spice has to solve such that KCL is satisfied, which usually means Ids*Vds = ΔT/rth.

The way you've written it looks like Verilog-A syntax, specifying that Pwr(T) is the current into the T node, which has to be zero by KCL -- unless you connect a thermal conductor to model heat transfer to a neighboring device.

Ids isn't an "unknown" -- once you know the node voltages, it's directly computable.

There are more than 2 unknowns -- V(d), V(g), V(s), etc. are all unknown.  I guess if you start with a non-self-heating model and assume that all the equations and unknowns work out (which they do), then when you go and add self-heating you're adding 1 unknown (ΔT) and one equation (KCL for the T node).