S parameter extraction for MOSFET internal parameters
Ofcourse the equations are not accurate but there is lot of error between the two. For example cgs i get from equations is 400 fF and from DC operation point is 96 fF (as far as i remeber, I will check and confirm again).
Can somebody comment this. How far these equations are valid and when to use these and when not. And how to jusify the error. Thanks
Can you understand what model you use for MOSFET in simulation ?
Is it BSIM3 or BSIM4 ?
If equations are correctly for your model, simulation results will be matched to calculations.
Surely learn very basic things before EDA Tool Play.
I am not sure, where/how do I verify which model it is?
See simulation model files.
Surely learn very basic things before EDA Tool Play.
400f and 96f are quite far apart. I have done similar measurements in bipolar transistors at 28GHz and 60GHz but it was never this far off.
Refer to the paper, "Parameter extraction technique for small signal equivalent circuit model of microwave silicon MOSFETs" from Lee and Yu. Are your expressions for the MOS internal parameters in your script/measurement setup same as that in the paper?
You do fundamental errors..
-DC OP gives you "static" intrinsic parameters, not dynamic..Briefly it computes intrinsic parameters for given DC OP.
-s-parameters relate the Input and Output to "small signal" Transfer Function under the condition Ports are terminated by Zo, so intrinsic parameters cannot be accurately extracted with s-parameters..
-Intrinsic Parameters can be extracted ONLY and ONLY by Modelling Softwares such as ICCAP etc. You measure the active device, you obtain DC,AC,s-parameters,Load Pull Values then that software extracts the intrinsic parameters in a certain tolerance accuracy in according to given model.
This needs an experienced engineering knowledge.
Model variations of BJT are not so many compared to MOSFET.
And capacitance models are very simple and easy.
(1) Gummel-Poon
(2) VBIC
(3) Mextram
Almost Gummel-Poon.
It was HiCUM. Gummel Poon is quite limited for its use in a PA.
But I get what you are saying. I will check it in a CMOS process.
Actually this is the book name "Distributed Power Amplifiers for RF and Microwave Communications Narendra KumarAndrei Grebennikov" and those equations are given from MESFET or HEMT. They look similar to the equations provided in the paper "Parameter Extraction Technique For The Small-signal Equivalent Circuit Model Of Microwave Silicon MOSFET" . Also I made few mistakes while writing those equations in calculator. At the end, I think I see there is a match between equations and the values I get from DC operating point for some parameters.
I think what the OP is trying to refer to is that he is using s-parameter analysis in Cadence Spectre. During sp analysis, it also gives you two port Y and Z parameters which can be used to get a rough values of MOS internal parameters. For example I checked in a 45nm PTM CMOS process and it was close for Cgs and Cgd. When the spectre models are made by taking into account series resistance and inductances with the terminals (which becomes essential for mmwave), the approximate expressions are not that great.
I did not have access to ICCAP but I used a dirty trick to get somewhat accurate detailed models in ADS. I made a simple model myself and then used the parameter optimization to extract different MOS parameter values. I used a wide band s-parameter extraction (around the frequency of operation) from spectre, converted it into .s2p file and used it in ADS to optimize my crude model.
I don't want to sound mean, but anytime you have doubt on your calculator expressions, run it on a simple analogLib models and see if you get the correct values. It saves you effort and also helps in separating the real issue from EDA Tool Play issues. I myself have had made disastrous mistakes in the past.
This is really a good tip.