Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

Characterization values of a MOSFET in PDK

garvind25

Full Member level 3
Joined
Oct 28, 2012
Messages
161
Helped
0
Reputation
0
Reaction score
1
Trophy points
1,298
Activity points
2,927
Hi,



I am trying to start off designing with gpdk90. In order to know the model parameters, I ran a simulation in Cadence (6.1.5) with an nmos. Once the simulation was complete, I went to Results > Print >Model parameters. I selected the nmos and got the values printed. My queries are:

  • Is this the right way to get the values of µn/p of a transistor? I need these values for calculation.
  • If this is the right way, the value of U0 for nmos is printed as 20m. What will be the units pls?
  • The value of tox for nmos is printed as 2.33n. How to get the value of Cox?
  • How to print the value of λ? I could not find the keyword ‘LAMBDA’ printed in the form. Is it given as something else?
Initially, I had thought of getting the values from the model card. But the model card has a lot of devices that it was not practical for me to look into the 35 page doc (attached). I just need the values of µ , Cox, Vtho and λ to start off. Hence, looking forward to your responses.



Thanks and Regards,

Arvind Gupta
 

dick_freebird

Advanced Member level 5
Joined
Mar 4, 2008
Messages
7,835
Helped
2,228
Reputation
4,464
Reaction score
2,176
Trophy points
1,393
Location
USA
Activity points
62,809
Modern models are "empirical" and although many "classical" model params remain they are surrounded by numerous "fitting" params which bend things considerably, arbitrarily (often abused) and make a "gut" understanding much harder than an old LEVEL=3 model.

I might recommend instead that (if you trust the models fundamentally) you set up testbenches for a device geometry of interest, and extract the "classical" params from DC sweep data - extrapolated VT, then get k' from Id-Vd, then get u0 from (effective, and that's a fun one) and geometry and tox, in the basic way. You'll lose the geometry effects (which are most of the trouble) but lots of people end up using one or a couple of Ls in the end so....
 

garvind25

Full Member level 3
Joined
Oct 28, 2012
Messages
161
Helped
0
Reputation
0
Reaction score
1
Trophy points
1,298
Activity points
2,927
Thanks for the reply. I have a few additional queries regarding the characterization run:

What values of W and L should I take for the characterization runs? One of my friends advised me that since I will need long channel dimensions to avoid channel length modulation effect, I use large values of W and L in the characterization runs. Is it ok if I take L=400nm and W=1.6u? If not, how to select these values?

How to get the value of CLM coefficient (Lambda)? Should I take the slope of Id vs Vds curve? If so, for what Vgs value should I consider the curve for slope extraction?



Looking forward to your replies.

Arvind Gupta
 

dick_freebird

Advanced Member level 5
Joined
Mar 4, 2008
Messages
7,835
Helped
2,228
Reputation
4,464
Reaction score
2,176
Trophy points
1,393
Location
USA
Activity points
62,809
Well, certainly min/min and 10u/10u are corners of
a sensible "box" (provided you mean to limit FET
finger W to that 10u; otherwise move the goalposts).
10/min and min/10. Dense series of L increment and
W increment near the minimum, something like a log
taper out to where you expect analog to end up.
Digital will live at the min L moderate W, RAM at min/min
or even cheat those. Seeing what a subminimum
device looks like can offer confidence (or warning).

This is all subject to gross technology influences
when you get to stuff like fin technologies where
there's only one size, use however many you like.
Creepy.

If you're thinking about RF then you want some
help from somebody who knows the best way to get
at devices and design those pad cages right, and
back all that baggage out of the model pull. DC
is easy. RF devices may be so difficult to fit that
only a few "unit geometries" are supported and
characterized from big arays that help swamp the
test environment influences. But maybe reticle
area is not free (it is for foundry technology
development engineering, sort of) and then you
might really have to focus on how to get whatever
it is you really need, for minimum effort and expense.
--- Updated ---

re lambda fitting, you want a model that is right for the
range of current densities that you expect anyone to
run. I'd say to look at decades, and bias the gate with
a replica network that puts another FET exactly where
you want it (say, 1uA at Vds=1.25V) by feedback, and
tap that replica FET's gate via vcvs to bias your lambda
extract device for the drain sweep. Step reference current
into the replica, get family of curves, etc.
 
Last edited:

LaTeX Commands Quick-Menu:

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Top