The Designer's Guide Community Forum

The Designer's Guide Community Forum
https://designers-guide.org/forum/YaBB.pl
Design Languages >> Verilog-AMS >> Transient Effect
https://designers-guide.org/forum/YaBB.pl?num=1408164288

Message started by Mirwazul Islam on Aug 15^th, 2014, 9:44pm

Title: Transient Effect
Post by Mirwazul Islam on Aug 15^th, 2014, 9:44pm

Hi,

I am trying to include transient temperature effect in Verilog. I haven't found dt function in any manual. How can i include transient temperature or any transient effect in Verilog? I would be glad if anyone can help me with this.

Thanks

Title: Re: Transient Effect
Post by Geoffrey_Coram on Aug 21^st, 2014, 2:52pm

What do you mean by transient temperature effect? Self-heating? Or that feature in some simulators that allows you to change the circuit ambient temperature step-wise during a transient analysis?

Title: Re: Transient Effect
Post by MMI on Aug 21^st, 2014, 9:57pm

Yes, self heating. I was searching this and got some idea from how they do it in MOSFET. I have created a module for parallel RC circuit with pulsed current input and measured output voltage. The output voltage corresponds to temperature, but i don't know yet how to incorporate that in my actual HFET model. Do you know any better way to do this?

Thanks

Title: Re: Transient Effect
Post by Geoffrey_Coram on Sep 23^rd, 2014, 2:29pm

Is your HFET model written in Verilog-A? There are a couple open-source models written in Verilog-A that include self-heating; it would be easy to copy their approach. (Mextram, Hicum, BSIMSOI, HiSIM-HV, ...)

Title: Re: Transient Effect
Post by Peng_Li on Mar 15^th, 2017, 12:14am

Geoffrey_Coram wrote on Sep 23^rd, 2014, 2:29pm:

Hi, Mr. Coram. I am recently using Verilog-A and Hspice to do electrical-thermal co-simulation, and interested in how they are implemented in other models.
As you suggested, I read the source code of Mextram and Hicum, focusing on their implementation of self-heating. There are two problems I do not quite understand.

1. The parameter system function, $temperature, is used. According to "Verilog-AMS Language Reference Manual", it returns the circuit’s ambient temperature in Kelvin units.
My question is: where is that temperature assigned?
For an HSPICE simulation, the command ".TEMPERATURE" is used to specify the circuit temperature. Is this what I am looking for?

2. Is self-heating calculation only conducted once?
In most literature about the loosely-coupled algorithm between electrical and thermal fields, convergence is obtained by iteration between the two analysis.
In the “Mextram” model, I couldn’t find any iteration between electrical analysis and thermal analysis. So I wonder if the self-heating effect is taken into account and conducted only once in the model.
In the “Hicum” model, a while() loop statement is used only to iterate for improved initial solution of total hole charge. Also, no iteration between electrical analysis and thermal analysis is found.
Could you give me some hint about how the self-heating is treated in these models?

Any help would be greatly appreciated.

Title: Re: Transient Effect
Post by Geoffrey_Coram on Mar 15^th, 2017, 9:55am

1. Yes, $temperature is the .temp in HSpice (or option tdegc in Spectre), though in Kelvin rather than Celsius

2. In those models, you should see something like
thermal dt;
which declares a "node" or unknown in the system of equations, and then the temperature of the device should be $temperature + Temp(dt), and that device temperature is used to update parameters and in the kT/q expression in the exponentials.
At the bottom of the model, you should see a calculation of dissipated power, which is used in a self-heating equivalent circuit: a current source of value Pdiss, a "thermal resistor" Rth, and a "thermal capacitance"Cth.
Self-heating is then computed self-consistently: the simulator provides a guess for the temperature of "dt" just as it does for the node voltages, computes the equations, and sees if KCL and KVL are satisfied.