Manuals >Netlist Translator for SPICE & Spectre >Chapter 8: Translating a Model
Print version of this Book (PDF file) 		prevnext

BSIM2_Model:BSIM2 MOSFET Model

The SPICE BSIM2 MOSFET model is translated to the ADS MOSFET BSIM2_Model. For translation information on the MOSFET device, refer to MOSFET Device.

For more information on the ADS model, place the model in a schematic and choose Edit > Component > Edit Component Parameters to view the model parameters. You can also click Help in the component editor dialog box for additional information.

Example SPICE Command Line: 
.model nch nmos level=39 rsh=0 js=0
SPICE Dialect and Netlist Syntax:

Spice2/3:

.model mname NMOS | PMOS LEVEL=5 [param=value]*

PSpice:

Does not exist

HSpice:

.model mname NMOS | PMOS LEVEL=39 [param=value]*

ADS Netlist Syntax:

model mname MOSFET NMOS=[0|1] PMOS=[0|1] Idsmod=5 [param=value]*

ADS Schematic Symbol:

Model Parameters:

For information on parameter format, refer to Using Parameter Mapping Tables to Understand a Translation.

Table 8-18. BSIM2_Model Parameters
ADS
Unit
Default
Spice2/3
HSpice
Idsmod

5
 Level=5
 Level=39
Rsh

0.0
 x
 x
Js
 A/m2
 0.0
 x
 x
Mu0
 cm2/V-s
 600
 x
 Def=400
Dl
 m
 0.0
 x
 x
Dw
 m
 0.0
 x
 x
Vdd
 V
 5.0
 x
 x
Vgg
 V
 5.0
 x
 x
Vbb
 V
 -5.0
 x
 x
Temp
 oC
 25
 x
 -
Tox
 m
 1e-7
 x
 x
Cj
 F/m2
 5.0
 x
 Def=0
Mj

0.5
 x
 x
Cjsw
 F/m
 0.0
 x
 x
Mjsw

0.33
 x
 x
Pb
 V
 0.8
 x
 x
Pbsw
 V
 1.0
 x
 Def=PB
Cgso
 F/m
 0.0
 x
 x
Cgdo
 F/m
 0.0
 x
 x
Cgbo

0.0
 x
 x
Xpart

1.0
 x
 -
Vfb (L, W)
 V
 -0.1
 x
 Def=-0.3
Phi (L, W)
 V
 0.6
 x
 Def=0.8
K1 (L, W)
 V
 0.5
 x
 x
K2 (L, W)

0.0
 x
 x
Eta0 (L, W)

0.08
 x
 Def=0
Ua0 (L, W)
 1/V
 670.0
 x
 Def=0
U10 (L, W)
 m/V
 0.0
 x
 x
Mu0b (L, W)
 cm2/V2s
 0.0
 x
 x
Etab (L, W)
 1/V
 -0.07
 x
 Def=0
Uab (L, W)
 1/V2
 0.0
 x
 x
U1b (L, W)
 m/V2
 0.0
 x
 x
U1d (L, W)
 m/V2
 0.0
 x
 x
Mus0 (L, W)
 cm2/Vs
 600.0
 x
 x
Musb (L, W)
 cm2/V2s
 0.0
 x
 x
N0 (L, W)

0.5
 x
 x
Nb (L, W)
 1/V
 1.0
 x
 x
Nd ((L, W)
 1/V
 0.0
 x
 x
Mu20 (L, W)

0.0
 x
 x
Mu2b (L, W)
 1/V
 0.0
 x
 x
Mu2g (L, W)
 1/V
 0.0
 x
 x
Mu30 (L, W)
 cm2/V2s
 0.0
 x
 x
Mu3b (L, W)
 cm2/V3s
 0.0
 x
 x
Mu3g (L, W)
 cm2/V3s
 0.0
 x
 x
Mu40 (L, W)
 cm2/v3s
 0.0
 x
 x
Mu4b (L, W)
 cm2/v4s
 0.0
 x
 x
Mu4g (L, W)
 cm2/v4s
 0.0
 x
 x
Ub0 (L, W)
 1/V2
 0.0
 x
 x
Ubb (L, W)
 1/V3
 0.0
 x
 x
Vof0 (L, W)
 V
 0.0
 x
 x
Vofb (L, W)
 1/V
 0.0
 x
 x
Vofd (L, W)
 1/V
 0.0
 x
 x
Ai0 (L, W)

0.0
 x
 x
Aib (L, W)
 1/V
 0.0
 x
 x
Bi0 (L, W)
 V
 0.0
 x
 x
Bib (L, W)

0.0
 x
 x
Vghigh (L, W)

V

0.0

x
 x
Vglow (L, W)
 V
 -0.15
 x
 Def=0

Comments:

Tox > 1 is in angstroms in HSpice. Translator will convert it to um.

For HSpice and ADS, most parameters have associated width and length sensitivity parameters. Consult your HSpice manual or refer to the ADS Circuit Components manual for more information.

ADS does not support NRD, RDC, NRS or RSC MOSFET parameters. If RD or RS are not given, they will be calculated as follows:

RD=NRD*RSH+RDC

RS=NRS*RSH+RSC

prevnext