Continue to Site

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.

Register Log in

How to determine K'p and K'n?

Status
Not open for further replies.
S

snoop835

Advanced Member level 4
Full Member level 1
Joined
Feb 7, 2005
Messages
102
Helped
6
Reputation
12
Reaction score
3
Trophy points
1,298
Location
Penang, Malaysia
Activity points
1,371
µn in tsmc 0.18 µm cmos

How do we determine the value for K'p of PMOS and K'n of NMOS? I have tried to look at the model parameters, but I don't know which parameter to choose. In the model parameter, they only stated K1, K2 and K3 but not K'n or K'p.

Another way, I run DC Sweep on a single transistor and get Vgs-Id curve, determine the linear slope, calculate K'p by using formula m=(k'pW/2L)1/2. This method is explained in P.E. Allen books. but I doubt my result is correct.

Pls throw me some light on this.

Thanks in advance

-snoop835-
 

what kind you the model? if hspice, you can refer to the mannul of hspice
 

Hi Sunking,

It's a BSIM3v3, HSPICE Level=49. But when I look at the HSPICE model parameter, I couldn't find Kp or Kn. They only specify for Threshold Voltage parameters, K1, K2 and K3. I doubt this is the parameter that i'm looking for.
 

in spice model, you can find U0, that is un or up.
 

Well I've seen it before, you better check on the topic of technology scaling. I don't quite remember but i believe it's a product from the transconductance(β) and something else.

But I'm quite sure you will find the answer under the topic of scaling,maybe try Uyemura books of "Introduction to VLSI"
 

snoop835,

K'n = 3K'p because µn = 3µp

Transconductance Process Parameter, K' = µCox
Capacitance Per Unit Area, Cox = ε/tox

E-mail to check with your foundry (TSMC, UMC, CSM, etc). Either they provide a chart/graph or tabulated values to use for tox and µ for specific technologies like 0.18, 0.13 µm etc.

µ must be provided because 0.18, 0.13 etc are short-channel devices.

Relative dielectric permittivity = ε is 4.5 for SiO2.

BTW, you should know all these before you graduated from universities.
 

    S

    snoop835

    Points: 2
    Helpful Answer Positive Rating
good work skyhigh
but for SiO2 ε=εox*ε0=3.9*8.854e-14F/cm=3.46e-11F/m
from tsmc0.18 hspice model, tox(nch)~=4e-9m tox(pch)~=4-9m,
un~=0.045m^2/v-s,up~=0.01m^2/v-s
so K'p=1/2*un*Cox=0.5*0.045*3.46e-11/4e-9=194.6uA/V
K'n=0.5*0.01*3.46e-11/4e-9=43.25uA/V

You can calculate K'p and K'n of pch3 and nch3 in the same way.
In fact, un and up vary slightly with W and L, but it doesn't matter to estamite K'p and K'n .
 

    S

    snoop835

    Points: 2
    Helpful Answer Positive Rating
    V

    Points: 2
    Helpful Answer Positive Rating
yes, SkyHigh and flushrat have show a method to caculate the Kp and Kn.

And you can run the dc simulation under artist to print dc operation points under the menu result
 

Acknowledged helps from members of forum i.e. sunking, flushrat and skyhigh. :)

cheers

-snoop835-
 

I think these parameter are supplied by foundry
 

snoop835 said:
How do we determine the value for K'p of PMOS and K'n of NMOS? I have tried to look at the model parameters, but I don't know which parameter to choose. In the model parameter, they only stated K1, K2 and K3 but not K'n or K'p.

Another way, I run DC Sweep on a single transistor and get Vgs-Id curve, determine the linear slope, calculate K'p by using formula m=(k'pW/2L)1/2. This method is explained in P.E. Allen books. but I doubt my result is correct.

Pls throw me some light on this.

Thanks in advance

-snoop835-
Click to expand...

K1, K2, and K3 approximates threshold voltage. In other hand, you may get Kp or Kn, taking U0 and eps-si, with oxide thickness. However, this only works for linear region.
 

sunking said:
yes, SkyHigh and flushrat have show a method to caculate the Kp and Kn.

And you can run the dc simulation under artist to print dc operation points under the menu result
Click to expand...

Can anyone tell me how to run the DC simulation to get K'p and K'n?
 

K'p and K'n are called KF in spice model
 

Kp and Kn are too rough to use for simulation, so they are really not used in anything but the lowest levels of spice models. You should simply calculate it as u*Cox as flushrat has done in his example.
 

simulating and getting these parameter are the best way.bsim3v3 model files don't give these parameters directly.
 

u may get these parameters from your foundry. good luck.
 

Answer ti this question can be found in every CMOS book but if you don't have any at your hands check the following tutorial: h**p://www.odyseus.nildram.co.uk/RFIC_Theory_Files/MOS_Transistor.pdf
 

Status
Not open for further replies.

Similar threads

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Back
Top