The Designer's Guide Community Forum

The Designer's Guide Community Forum
https://designers-guide.org/forum/YaBB.pl
Simulators >> Circuit Simulators >> Help needed for understanding model parameters
https://designers-guide.org/forum/YaBB.pl?num=1224649674

Message started by kidman on Oct 21^st, 2008, 9:27pm

Title: Help needed for understanding model parameters
Post by kidman on Oct 21^st, 2008, 9:27pm

I got a design kit but I can't really find the parameters im looking for in the device model. Below is the device model parameters. The parameters I'm looking for are
1- GAMMA
2- LAMBDA
3- PHI
Excuse my ignorance...I'm still a beginner

*****Model Selectors/Controllers*********************************
+ LEVEL = 4.9000E+01 VERSION = 3.2400E+00
+ BINUNIT = 2.0000E+00 MOBMOD = 1.0000E+00
+ CAPMOD = 3.0000E+00 NQSMOD = 0.0000E+00
+ NOIMOD = 2.0000E+00
*****Process Parameters******************************************
+ NGATE = 7.6755E+20 RSH = 9.0000E+00
+ TOX = '7.1300E-09+DTOX_N_HGLVBPW_33_L130E' TOXM = 7.1300E-09
+ XJ = 1.0500E-07 NCH = 9.7100E+16

*****Basic Model Parameters**************************************
+ VTH0 = '1.8602E-01+DVTH0_N_HGLVBPW_33_L130E' VFB = -1.2758E+00
+ K1 = 6.6000E-01 K2 = 0.0000E+00
+ K3 = -4.4000E+00 K3B = 0.0000E+00
+ W0 = 3.9100E-07 NLX = 2.1800E-07
+ DVT0 = 1.2867E+00 DVT1 = 4.7170E-01
+ DVT2 = -1.8700E-01 DVT0W = 1.2250E+00
+ DVT1W = 1.2398E+07 DVT2W = -3.8770E-01
+ U0 = '3.5220E-02+DU0_N_HGLVBPW_33_L130E' UA = -8.0190E-11
+ UB = 1.4520E-18 UC = 5.0000E-11
+ VSAT = '9.7500E+04+DVSAT_N_HGLVBPW_33_L130E' A0 = 8.0000E-01
+ AGS = 3.0100E-01 B0 = 9.4300E-06
+ B1 = 2.6900E-05 KETA = -5.0000E-03
+ A1 = 0.0000E+00 A2 = 9.1000E-01
+ WINT = '5.5600E-08+DWINT_N_HGLVBPW_33_L130E' LINT = '2.5850E-08+DLINT_N_HGLVBPW_33_L130E'
+ DWG = -1.8000E-09 DWB = 1.2100E-09
+ VOFF = -1.2173E-01 NFACTOR = 1.2000E+00
+ ETA0 = 1.2250E-01 ETAB = -3.0000E-01
+ DSUB = 1.3559E+00 CIT = 8.5000E-04
+ CDSC = 0.0000E+00 CDSCB = 0.0000E+00
+ CDSCD = 1.0000E-04 PCLM = 1.3250E+00
+ PDIBLC1 = 1.0000E+00 PDIBLC2 = 3.0400E-03
+ PDIBLCB = 1.0000E-01 DROUT = 1.0000E+00
+ PSCBE1 = 7.0300E+09 PSCBE2 = 3.5000E-03
+ PVAG = 6.0000E-01 DELTA = 1.0000E-03

*****Parameters for Asymmetric and Bias-Dependent Rds Model******
+ RDSW = '3.8917E+02+DRDSW_N_HGLVBPW_33_L130E' PRWB = 5.3200E-02
+ PRWG = 6.5000E-02 WR = 1.0000E+00

*****Impact Ionization Current Model Parameters******************

*****Gate-Induced Drain Leakage Model Parameters*****************

*****Gate Dielectric Tunneling Current Model Parameters**********

*****Charge and Capacitance Model Parameters*********************
+ XPART = 1.0000E+00 CGSO = '3.9100E-10+DCGSO_N_HGLVBPW_33_L130E'
+ CGDO = '3.9100E-10+DCGDO_N_HGLVBPW_33_L130E' CGBO = 0.0000E+00
+ CGSL = 0.0000E+00 CGDL = 0.0000E+00
+ CKAPPA = 6.0000E-01 CF = 0.0000E+00
+ CLC = 1.0000E-07 CLE = 6.0000E-01
+ DLC = 8.2000E-08 DWC = 0.0000E+00
+ VFBCV = 0.0000E+00 NOFF = 1.9996E+00
+ VOFFCV = -5.1000E-02 ACDE = 3.8556E-01
+ MOIN = 2.6250E+00

*****High-Speed/RF Model Parameters******************************

*****Flicker and Thermal Noise Model Parameters******************
+ NOIA = 9.2795E+20 NOIB = 5.9591E+04
+ NOIC = -1.0000E-15 EF = 0.8928
+ EM = 2.6493E+07

*****Layout-Dependent Parasitics Model Parameters****************
+ XL = 0.0000E+00 XW = 0.0000E+00

*****Asymmetric Source/Drain Junction Diode Model Parameters*****
+ JSW = 1.0000E-12 JS = 8.8000E-07
+ IJTH = 1.0000E-01 CJ = '9.7100E-04+DCJ_N_HGLVBPW_33_L130E'
+ MJ = 3.5800E-01 MJSW = 2.3000E-01
+ CJSW = '1.0500E-10+DCJSW_N_HGLVBPW_33_L130E' CJSWG = '9.0000E-11+DCJSWG_N_HGLVBPW_33_L130E'
+ MJSWG = 5.0000E-01 PBSW = 6.0000E-01
+ PB = 6.9100E-01 PBSWG = 6.2000E-01

*****Temperature Dependence Parameters***************************
+ TNOM = 2.5000E+01 UTE = -1.4650E+00
+ KT1 = -3.6500E-01 KT1L = 2.8000E-09
+ KT2 = -3.2000E-02 UA1 = 3.9700E-10
+ UB1 = -1.1000E-18 UC1 = -1.0000E-10
+ PRT = -1.6400E+02 AT = 3.3600E+04
+ XTI = 3.0000E+00 TPB = 1.4700E-03
+ TPBSW = 5.9700E-04 TPBSWG = 4.8000E-03
+ TCJ = 8.8000E-04 TCJSW = 7.9600E-04
+ TCJSWG = 1.2000E-02

*****dW and dL Parameters****************************************
+ WL = -1.1100E-14 WLN = 1.0000E+00
+ WW = -6.0000E-15 WWN = 1.0000E+00
+ WWL = 1.1100E-21 LL = -3.1250E-17
+ LLN = 1.0000E+00 LW = -2.2700E-15
+ LWN = 1.0000E+00 LWL = 7.7500E-26
+ LLC = -8.8000E-15 LWC = 0.0000E+00
+ LWLC = 0.0000E+00 WLC = 0.0000E+00
+ WWC = 0.0000E+00 WWLC = 0.0000E+00

*****Range Parameters for Model Application**********************
+ LMIN = 3.4000E-07 LMAX = 5.0000E-05
+ WMIN = 1.6000E-07 WMAX = 1.0000E-04

*****Other Parameters********************************************
+ ELM = 5.0000E+00 ACM = 1.2000E+01
+ LDIF = 9.0000E-08 HDIF = 1.3400E-07
+ CALCACM = 1.0000E+00 LVTH0 = '-1.0118E-08+DLVTH0_N_HGLVBPW_33_L130E'
+ WVTH0 = '1.2000E-09+DWVTH0_N_HGLVBPW_33_L130E' PVTH0 = '-4.0600E-16+DPVTH0_N_HGLVBPW_33_L130E'
+ PK2 = 1.2817E-15 PVSAT = '1.0000E-11+DPVSAT_N_HGLVBPW_33_L130E'
+ LUA = -6.9514E-18 LUB = 3.3537E-26
+ PUB = -5.0000E-32 PUC = -4.5000E-24
+ WU0 = '-6.3600E-11+DWU0_N_HGLVBPW_33_L130E' PU0 = '1.1000E-18+DPU0_N_HGLVBPW_33_L130E'
+ LKETA = 6.8000E-10 LVOFF = -3.0000E-09
+ LNFACTOR = 4.5000E-08 PNFACTOR = -8.0000E-15
+ PDSUB = 1.9800E-14 PPDIBLC2 = 7.6000E-16
+ LDELTA = 7.5800E-09 PKT1 = 7.5000E-16
+ LKT2 = 3.9004E-09 PAT = -1.4300E-10
+ WUTE = 4.1790E-08 PUTE = -2.0000E-15
+ WUB1 = 1.1600E-25 PUB1 = 2.0000E-33
+ PUC1 = 3.0000E-24

*****User Drop Parameters****************************************

*****High-Speed/RF Model Parameters******************************

Title: Re: Help needed for understanding model parameters
Post by Geoffrey_Coram on Oct 22^nd, 2008, 6:43am

kidman wrote on Oct 21^st, 2008, 9:27pm:

Those parameters are for the original MOS models built into Spice3 in the 70s or 80s (LEVEL=1 to 3). The model card you show is BSIM3, which is much more advanced.

Often, in classes, the simple MOS-1 or 3 equations will be used so you can get an intuitive feel for how the device works. However, these equations aren't adequate to accurately describe the currents and charges in modern semiconductor processes.

Title: Re: Help needed for understanding model parameters
Post by kidman on Oct 22^nd, 2008, 12:00pm

Thanks Geoffrey. But what do you think I should do? I am studying from Berkeley webcasts and Razavi's book and both use the old parameters. What do you think I should do ?

Title: Re: Help needed for understanding model parameters
Post by didac on Oct 22^nd, 2008, 12:40pm

Hi,
I think you have two options:
1)if it's just for learning purposes and you don't really care about the accuracy(not intended for silicon manufacturing) you can take a look at MOSIS, they provide SPICE models from their processes(I suppose it's what it's used in the webcasts), there are several processes to choose:
http://www.mosis.com/Technical/Testdata/menu-testdata_mep.html.
2)A rough approximation with the model that you have: formulate the standard square-law equation and isolate the variables that you want to estimate-with some assumptions because you will find Vth and lambda all together-, perform DC simulations and calculate the values. After hand calculation you can see how much divergence exist between hand calculation and the square law model. As a reference I remember:http://personalpages.to.infn.it/%7Ecobanogl/lowlevelstuff/tutparext and http://personalpages.to.infn.it/%7Ecobanogl/lowlevelstuff/tutparext2.
As Geoffrey said modern processes doesn't fit the standard equation, so this results(1 or 2) are only approximations for quick math, final circuits must be tunned using simulations.
Hope it helps,
edit:MOSIS don't provide LAMBDA, my memory it's starting to fail...

Title: Re: Help needed for understanding model parameters
Post by didac on Oct 23^rd, 2008, 12:46am

Hi,
Looking again at MOSIS SPICE models I remembered that LAMBDA in this level it's embedded through KAPPA parameter, with a couple of equations that model modifies effective channel length to include channel length modulation.
Hope it helps,

Title: Re: Help needed for understanding model parameters
Post by Geoffrey_Coram on Oct 23^rd, 2008, 4:45am

LAMBDA appears to be a LEVEL=1 parameter. What are you trying to do? If you just need a set of parameters, then didn't you get some in the lecture material? You at least should have some order of magnitude values -- eg, LAMBDA=0.1 -- so you can vary that to 0.05 or 0.2 and see what happens. You can also start with the MOSIS values, ignore the ones that aren't used in LEVEL=1 (KAPPA, etc.) and add LAMBDA=0.1 just to see what it does.

Title: Re: Help needed for understanding model parameters
Post by kidman on Oct 24^th, 2008, 1:14am

What I am trying to do is as follows:

The lecture material has a design project to be made ( a simple Op-Amp) and I happen to have the Cadence IC and Virtuoso program and some foundry's design kit. So I am trying to get the parameters I need for hand calculations from the models included in the kit, do my design, then simulate it. It's a 0.13u kit. I really don't know anything about SPICE in general...I know nothing about netlists and so, I can only simulate simple circuits in Pspice for college work. I was advised not to waste my time on learning SPICE and how to write netlists because I have Cadence tools. What do you think?