Dear Naveen,
There are two main questions you have to ask yourself in order to find
the best model for your application :
1. What is your application ? what do you want to model or simulate ?
What is the more accurate model for your design needs ?
You've already answered this question => MOS subthreshold region,
which is a good start.
2. Is your foundry, Model or PDK provider can supply you the model you
need ? That's im****tant as well !
back to your questions :
1. BSIM3v3 is the industry standard nowadays, it has a very good
modeling of the Sub-threshold region and it is sup****ted and provided
by almost all the foundries.
BSIM4 is getting more popular among the nano technologies world since
it is solving many missing items from the BSIM3, such as the Well
Proximity Effect (WPE), the Shallow Trench Isolation stress (STI),
Halo/Pocket modeling, Gate direct Tunneling, GIDL ... Except these new
silicon side effects at small geometries, i don't think BSIM4 has
improved anything directly related to the sub-threshold region. So do
you really need the modeling of these new stuffs ? what is your
technology node ? If you're in 0.13u and below, I would say BSIM3 is
fair enough.
Apart from BSIM3, PSP has been selected as a standard for nano
technologies by the Compact Modeling Council group, but do you really
need it ? This is a re****t from TI about sub-Threshold modeling in
PSP ...
http://www.eigroup.org/CMC/next_gen_cmos/phase3/ti.pdf
PSP is getting more power among the semiconductor wold but only few
foundries are sup****ting it now ...
Well, there are other modeling standards but my knowledge of EKV,
HiSIM and stuff is very very weak.
If you fancy reading about modeling, I would advice :
1. The CMC's (Compact Modeling Council) web site:
http://www.geia.org/index.asp?bid=597
2. The BSIM's web site
http://www-device.eecs.berkeley.edu/~bsim/
3. The following books:
3.1 Device Modeling for Analog and RF CMOS Circuit Design (Book)
3.2 Operation and Modeling of the MOS Transistor MOSFET
3.3 Models for SPICE Simulation, Including BSIM3v3 and BSIM4
2. I entirely commit with Stefan, you've to be a bit nosy ... File
searching in Unix is not harmful. search your PDK for .scs
(spectre), .lib (Eldo, Hspice), .gem (ADS) ...
3. These parameters are in your Spice Model Cards, and sometimes
supplied in foundry's do***entation (few set of them).
For your question : "But my question is where is that technology
file", my answer is : give me the IP address of your machine, your
username and your password, shut down all the firewalls and other
security stuffs. I'll then log on and give you the answer. You will be
certainly fired for this ;-) Nobody can answer this question my
buddy ! it depends on your PDK provider. Some BAD foundries even
change the locations from a pdk version to another ...
Well I'm not that bad and I can say that your simulator can dump these
parameters for you. You just need to make a test bench with one single
transistor, biased with DC voltage sources and run a DC OP simulation.
Go to the ADE -> Results -> Print -> Model Parameters and then select
your MOS !! This is what I propose to begin with. There are other ways
to do it if requested.
Hope this is helping you !
Riad.
|
