mosfet model spice/pspice

Hello Robin,

Even though it says level 3 model, it is missing lots of level 3 model parameters such as GAMMA (the bulk threshold parameter), the Sheet Resistance(RSH), lateral diffusion length (LD), the bulk junction potential (PB), 

the surface mobility (U0), and the capacitances, CGSO, CGDO, CJSW, CJ and without these values specified it will take on the default values.  

Robin,

U0 is in the model file (I believe U0 and UO are aliases) - however, Spectre reports that there's an inconsistency between kp and uo.

Notice from spectre during initial setup.
PMOS: Values of `kp' and `uo' are not consistent.
PMOS: `cgso' is not specified. 0.1um * Cox is used.
PMOS: `cgdo' is not specified. 0.1um * Cox is used.

Anyway, what I did to check was the following:

// pick one or the other
pspice_include "forum75mod.sp"
//include "forum75mod.sp"

M1 (d g vdd vdd) PMOS w=10u l=2u
Vdd (vdd 0) vsource dc=5
Vd (d 0) vsource dc=3
Vg (g 0) vsource dc=3

dc dc
models info what=models where=file

This produced forum75.info.models which listed the model parameters, and I did a diff:

UNIX> diff forum75.info.models_spectre forum75.info.models_pspice
13c13
< uo = 459.583 Mcm^2/V*s
---
> uo = 600 cm^2/V*s
124c124
< compatible = spectre
---
> compatible = pspice

So the difference is in the compatibility layer for MOS3 related to how UO is handled. Whilst the model is not specifically for PSPICE, the chances are it is for a SPICE typically used for discrete devices and those are likely to be compatible with PSPICE.

Regards,

Andrew.

Andrew,

Thanks. The value 600 cm^2/V*s for uo seems to be a spice default for this value. I tried removing KP and/or U0 from the model and setting U0 to 600 but I couldn't get the correct behaviour so I shall just carry on treating it as a pspice model.

Regards,

Robin

Robin,

That would generally be my advice when using a SPICE model of a discrete component; usually using PSPICE compatibility mode is the best solution then.

Regards,

Andrew.

Hi Robin,

In addition, I looked in the Spectre Circuit Simulator Components and Device Models Reference manual (<SPECTREinstDir>/doc/spectremod/spectremod.pdf) in the Common MOSFET Equations chapter (chapter 12). There's a section Parameters Common to Levels 1-3 Only which (near the end of that section, on page 1033/1034 in SPECTRE181 or 1034/1035 in SPECTRE191) which describes what happens when both uo and kp are specified, and the difference between spectre and other SPICE simulators (it doesn't explicitly mention PSPICE, because PSPICE compatibility is more recent than the model manual has been updated, but it's similar).

Hope that helps too,

Andrew.

Hi Andrew,

That gave me some idea of what is going on. I think Vdsat modelling is involved as the Vdsat value in the simulator was 2e-5 when I treated it as a spice model. Setting VMAX=3e12 in the model gave approximately the right behaviour but could have other effects so I will stick with using the original model as a Pspice model.

Thanks,

Robin

Hi Andrew,

That gave me some idea of what is going on. I think Vdsat modelling is involved as the Vdsat value in the simulator was 2e-5 when I treated it as a spice model. Setting VMAX=3e12 in the model gave approximately the right behaviour but could have other effects so I will stick with using the original model as a Pspice model.

Thanks,

Robin