Menu
▾
▴
Re: [Ngspice-users] TMSC 0.18 micron model parameter
|
From: Victor B. <bou...@ma...> - 2007-04-20 16:10:57
|
Hi, Given the absolute deluge of questions to this e-mail list, I decided to install NGSPICE and run some tests :) to Vimal : it is difficult to tell what is the problem without further information. How are your TSMC parameters are specified? For what model? Is it BSIM3v3.x? Suppose you take the parameters from http://www.ee.ucla.edu/~ingrid/Courses/ee215b/Handouts/t18h_lo_epi-params-mod.txt I did that, and made a very simple circuit file, as follows: ----------bsim3.cir--------------- *Simple Circuit to do Ids-Vgs simulations VDS 1 0 0.1 VGS 2 0 0 VBS 3 0 0 .DC VGS 0.0 2.0 0.1 M1 1 2 0 3 NMOD L=0.18u W=0.5u .MODEL NMOD NMOS LEVEL = 8 hdif = 0.25e-6 acm = 3 +VERSION = 3.2 TNOM = 27 TOX = 4.2E-9 +XJ = 1E-7 NCH = 2.3549E17 VTH0 = 0.3710619 +K1 = 0.5940793 K2 = 2.070131E-3 K3 = 1E-3 +K3B = 2.7158495 W0 = 1E-7 NLX = 2.005089E-7 +DVT0W = 0 DVT1W = 0 DVT2W = 0 +DVT0 = 1.4615376 DVT1 = 0.3798134 DVT2 = 0.0692378 +U0 = 293.522312 UA = -6.73646E-10 UB = 1.164182E-18 +UC = -2.84532E-11 VSAT = 9.286324E4 A0 = 1.7591856 +AGS = 0.3162202 B0 = -5.950938E-8 B1 = -1E-7 +KETA = 0.0111532 A1 = 3.896574E-4 A2 = 1 +RDSW = 139.0465393 PRWG = 0.5 PRWB = -0.2 +WR = 1 WINT = 0 LINT = 9.265899E-9 +XL = -2E-8 XW = -1E-8 DWG = -1.343579E-9 +DWB = -1.391607E-8 VOFF = -0.0765575 NFACTOR = 2.4791597 +CIT = 0 CDSC = 2.4E-4 CDSCD = 0 +CDSCB = 0 ETA0 = 0 ETAB = -0.0608407 +DSUB = 1 PCLM = 0.8853499 PDIBLC1 = 0.116863 +PDIBLC2 = 0.01 PDIBLCB = -0.0475298 DROUT = 0.5922434 +PSCBE1 = 8E10 PSCBE2 = 5.248199E-10 PVAG = 0.089248 +DELTA = 0.01 RSH = 6.8 MOBMOD = 1 +PRT = 0 UTE = -1.5 KT1 = -0.11 +KT1L = 0 KT2 = 0.022 UA1 = 4.31E-9 +UB1 = -7.61E-18 UC1 = -5.6E-11 AT = 3.3E4 +WL = 0 WLN = 1 WW = 0 +WWN = 1 WWL = 0 LL = 0 +LLN = 1 LW = 0 LWN = 1 +LWL = 0 CAPMOD = 2 XPART = 0.5 +CGDO = 7.75E-10 CGSO = 7.75E-10 CGBO = 1E-12 +CJ = 9.955315E-4 PB = 0.7345743 MJ = 0.3629904 +CJSW = 2.586055E-10 PBSW = 0.6451808 MJSW = 0.1296914 +CJSWG = 3.3E-10 PBSWG = 0.6451808 MJSWG = 0.1296914 +CF = 0 PVTH0 = 1.33957E-3 PRDSW = -5 +PK2 = -1.7189E-4 WKETA = 0.010864 LKETA = -0.0102793 +PU0 = 37.4749547 PUA = 1.762367E-10 PUB = 9.411793E-25 +PVSAT = 2E3 PETA0 = -1E-4 PKETA = -1.356792E-3 .END -------------end of bsim3.cir------------------ Running NGSPICE produced this: -----------test run ------------- $ ngspice bsim3.cir ****** ** ngspice-17 : Circuit level simulation program ** The U. C. Berkeley CAD Group ** Copyright 1985-1994, Regents of the University of California. ** Please submit bug-reports to: ngs...@li... ** Creation Date: Fri Apr 20 16:20:25 GMTST 2007 ****** winProcEstablishConnection - Hello winProcEstablishConnection - Clipboard is not enabled, returning. Circuit: *Simple Circuit to do Ids-Vgs simulations ngspice 1 -> run Doing analysis at TEMP = 300.150000 and TNOM = 300.150000 No. of Data Rows : 21 ngspice 2 -> plot vds#branch ngspice 3 -> quit Warning: the following plot hasn't been saved: dc1 *Simple Circuit to do Ids-Vgs simulations, DC transfer characteristic Are you sure you want to quit (yes)? y ngspice-17 done -----------end of test run ------------- Hope it helps in any way. Regards, Victor Mr T. Vimal P. Singh wrote: >Hello > >I tried to put device models in the form of .MODEL >CMOSN NMOS ( level=xx ...) using TSMC 0.18 parameters. >It returns that these model parameters are not >recognised. > >How should I do now? > >Vimal > >************************************************************************* >Vimal P. Singh Thoudam | Personal Web >Dept of EE, NERIST, Nirjuli, | www.nerist.ac.in/~vimal >Arunachal Pradesh, India | www.vimalprakash.cjb.net >(91) 360 2257850 (R) | (91) 94360 59445 >************************************************************************* > > |
