How to determine K'p and K'n?

[snoop835]

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-

 

[sunking]

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

 

[snoop835]

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.

 

[flushrat]

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

 

[Syukri]

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"

 

[SkyHigh]

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.

 

[flushrat]

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 .

 

[sunking]

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

 

[snoop835]

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

cheers

-snoop835-

 

[wjx197733]

I think these parameter are supplied by foundry

 

[mazelk]

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-

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.

 

[pugongying]

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

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

 

[kenlino]

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

 

[electronrancher]

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.

 

[shake2004]

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

 

[samuel]

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

 

[pirpana]

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