The BSIM3 version 2.0 MOS model from UC Berkeley is available as the LEVEL 47 Star-Hspice model.
The Star-Hspice LEVEL 47 model uses the same model parameters for source/drain diode current, capacitance, and resistance as do the other Star-Hspice MOS levels. The model parameter ACM controls the choice of source/drain equations.
The Star-Hspice LEVEL 47 model also uses the same noise equations as the other levels. The parameter NLEV controls the choice of noise equations.
This model, like all models in Star-Hspice, can be parametrized. This is useful for modeling process skew, either by worst-case corners or by Monte Carlo. For information on worst-case and Monte Carlo analysis, see Performing Worst Case Analysis and Performing Monte Carlo Analysis.
1. Set LEVEL=47 to identify the model as a BSIM3 model.
2. This model is based on BSIM3 version 2.0 from UC Berkeley. Code was received from UC Berkeley in July 1994, in the form of SPICE3e2. Changes announced in a letter from UCB September 13, 1994, have been included. DC sweeps have been checked against SPICE3e2.
3. The default setting for CAPOP is CAPOP=13, which is the BSIM1 charge-conserving capacitance model. The BSIM3 capacitance model has not been installed.
4. The LEVEL 47 model supports the model parameter name TNOM as an alias for TREF. The conventional terminology in Star-Hspice is TREF, which is supported as a model parameter in all Star-Hspice MOS levels. The alternative name TNOM is supported for LEVEL 47, for compatibility with SPICE3.
5. The default room temperature is 25°C in Star-Hspice, but is 27°C in SPICE3. If the BSIM3 model parameters are specified at 27°C, TREF=27 should be added to the model, so that the model parameters is interpreted correctly. It is a matter of choice whether or not to set the nominal simulation temperature to 27, by adding .OPTION TNOM=27 to the netlist. This should be done when testing Star-Hspice versus SPICE3.
6. The default of DERIV is zero, the analytical method. DERIV can be set to 1 for the finite difference method. The analytic derivatives in the SPICE3e2 code are not exact in some regions. Setting DERIV=1 gives more accurate derivatives (GM, GDS, GMBS), but consumes more CPU time.
7. There are three ways for the BSIM3 model to calculate Vth:
8. The model parameters NPEAK and U0 can be entered in meters or centimeters. NPEAK is converted to cm-3 as follows: if NPEAK is greater than 1e20, it is multiplied by 1e-6. U0 is converted to m2/Vsec as follows: if U0 is greater than 1, it is multiplied by 1e-4. You must enter the parameter NSUB in cm-3 units.
9. The specified value of VTH0 for p-channel in the .MODEL statement should be negative.
10. The default value of KT1 is -0.11. The negative sign ensures that the absolute value of threshold decreases with increasing temperature for NMOS and PMOS.
11. Model parameter LITL is not allowed to go below a minimum value of 1.0e-9 m, to avoid a possible divide by zero error.
12. VSAT, after temperature adjustment, is not allowed to go below a minimum value of 1.0e4 m/sec, to assure that it is positive after temperature compensation.
13. There are seven model parameters for accommodating the temperature dependencies of six temperature dependent model variables. They are KT1 and KT2 for VTH, UTE for U0, AT for VSAT, UA1 for UA, UB1 for UB, and UC1 for UC.
14. Set up the conversion of temperature between Star-Hspice and SPICE3 as follows:
15. The option SCALM does not affect the parameters unique to this model, but it does affect the common MOS parameters, such as XL, LD, XW, WD, CJ, CJSW, JS, and JSW.
16. LEVEL 47 uses the common Star-Hspice MOS parasitic models, specified by ACM.
17. LEVEL 47 uses the common Star-Hspice MOS noise models, specified by NLEV.
18. DELVTO and DTEMP on the element line can be used with LEVEL 47.
19. The impact ionization current determined by the model parameters PSCBE1 and PSCBE2 contributes to the drain-source current; it does not contribute to bulk current.
The standard Star-Hspice equations for Leff and Weff are:
The UCB SPICE3 equations used for BSIM3 are:
The units for these parameters are meters, with defaults of zero.
Star-Hspice uses the standard Star-Hspice equation for both cases, and accepting DL(DW) as the value for LD(WD). If both LD(WD) and DL(DW) are specified in an Star-Hspice .MODEL statement, Star-Hspice uses the LD(WD) value.
If LDAC and WDAC are included in the .MODEL statement,
Leff = L+XL-2·LDAC, Weff = W+XW-2·WDAC
The model uses the values of LD(DL) and WD(DW) to generate defaults for CGSO, CGDO, and CGBO. The values are also used with parameters RS and RD for ACM>0.
The following two models give the same Star-Hspice results:
.MODEL n1 nmos LEVEL=47 XL=0.1e6 LD=0.15e-6
+ SatMod=2 SubthMod=2 BulkMod=1
+ CGSO=0.3e-9 CGDO=0.3e-9 CGBO=0
.MODEL n2 nmos LEVEL=47 LD=0.1e-6
+ SatMod=2 SubthMod=2 BulkMod=1
+ CGSO=0.3e-9 CGDO=0.3e-9 CGBO=0
The following model equations are based on the source code of BSIM3.
If Phis is not specified as a model parameter, then
If K1, K2 are not specified as model parameters, then they are calculated as follows:
If Vbi is not specified as a model parameter, then
(if Pfactor > 1, it is set to Pfactor = 1)
Vdsat for the case Rds = 0 and Pfactor = 1:
Vdsat is the solution of Tmpa * Vdsat * Vdsat - Tmpb * Vdsat + Tmpc = 0
The following is an example of a PMOS model. Note that VTH0 is negative.
+ Npeak= 1.5E+23 Tox=7.0E-09 Xj=1.0E-07
+ SatMod= 2 SubthMod= 2 BulkMod= 1
+ Vth0= -.8 Phi= .7 K1= .5 K2=0.03 K3= 0
+ Dvt0= 48 Dvt1= .6 Dvt2=-5e-4
+ Vsat= 9E6 Ua= 1E-09 Ub= 0 Uc= -3E-02
+ Voff=-.07 NFactor= 1.5 Cit=-3E-05
+ Cdsc= 6E-02 Vglow=-.12 Vghigh= .12
+ Pclm= 77 Pdibl1= 0 Pdibl2= 2E-011
+ Drout= 0 Pscbe1= 0 Pscbe2= 1E-28
+ Ua1= 4E-09 Ub1= 7E-18 Uc1= 0
Star-Hspice Manual - Release 2001.2 - June 2001