The Designer's Guide Community
Forum
Welcome, Guest. Please Login or Register. Please follow the Forum guidelines.
Mar 28th, 2024, 7:11am
Pages: 1
Send Topic Print
Transient Effect (Read 4856 times)
MMI
New Member
*
Offline



Posts: 4
Columbia, SC, USA
Transient Effect
Aug 15th, 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
Back to top
 
 
View Profile   IP Logged
Geoffrey_Coram
Senior Fellow
******
Offline



Posts: 1998
Massachusetts, USA
Re: Transient Effect
Reply #1 - Aug 21st, 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?
Back to top
 
 

If at first you do succeed, STOP, raise your standards, and stop wasting your time.
View Profile WWW   IP Logged
MMI
New Member
*
Offline



Posts: 4
Columbia, SC, USA
Re: Transient Effect
Reply #2 - Aug 21st, 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
Back to top
 
 
View Profile   IP Logged
Geoffrey_Coram
Senior Fellow
******
Offline



Posts: 1998
Massachusetts, USA
Re: Transient Effect
Reply #3 - Sep 23rd, 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, ...)
Back to top
 
 

If at first you do succeed, STOP, raise your standards, and stop wasting your time.
View Profile WWW   IP Logged
Peng_Li
Junior Member
**
Offline



Posts: 10
Hangzhou, China
Re: Transient Effect
Reply #4 - Mar 15th, 2017, 12:14am
 
Geoffrey_Coram wrote on Sep 23rd, 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, ...)


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.
Back to top
 
 
View Profile   IP Logged
Geoffrey_Coram
Senior Fellow
******
Offline



Posts: 1998
Massachusetts, USA
Re: Transient Effect
Reply #5 - Mar 15th, 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.
Back to top
 
 

If at first you do succeed, STOP, raise your standards, and stop wasting your time.
View Profile WWW   IP Logged
Pages: 1
Send Topic Print
Copyright 2002-2024 Designer’s Guide Consulting, Inc. Designer’s Guide® is a registered trademark of Designer’s Guide Consulting, Inc. All rights reserved. Send comments or questions to editor@designers-guide.org. Consider submitting a paper or model.