PSPICE MOSFETS vs. Berekely SPICE3F5 MOSFETS

[Maxish]

Hello,

I have a model for a Motorola MOSFET - mtp6n60/mc. I get an error about several mosfet parameters (LAMBDA one of them) when trying to simulate it in Multisim- an XPICE/SPICE3F5 based simulator. The model is specified as a "Level 3" mosfet and according to SPICE3F5 specs, the error inducing parameters are not supported in level 3, so the error makes sense. In fact, no SPICE model level supports the set of parameters in my model. My guess is that this model is created specificaly for PSPICE or HSPICE who deviate from SPICE3F5 slightly.

Does anyone have a suggestion on how to simulate this model in basic Berkely SPICE3F5?

Here's the model:

.subckt mtp6n60/mc 10 20 30


* 10 = Drain 20 = Gate 30 = Source
*
******************************************************************************
*
*------------------------ EXTERNAL PARASITICS --------------------------------
* PACKAGE INDUCTANCE
*
LDRAIN 10 11 4.5e-09
LGATE 20 21 7.5e-09
LSOURCE 30 31 7.5e-09
*
* RESISTANCES
*
RDRAIN1 4 11 RDRAIN 0.8036
RDRAIN2 4 5 RDRAIN 0.0084
RSOURCE 31 6 RSOURCE 0.02018
RDBODY 8 30 RDBODY 0.0135
*
RGATE 21 2 5
*
*--------------------------------------------------------------------------
*
*--------------- CAPACITANCES AND BODY DIODE ------------------------------
*
DBODY 8 11 DBODY
DGD 3 11 DGD
CGDMAX 2 3 2.7e-09
RGDMAX 2 3 1e+08
CGS 2 6 1.31e-09
*
*--------------------------------------------------------------------------
*
*----------------------- CORE MOSFET --------------------------------------
*
M1 5 2 6 6 MAIN
*
*--------------------------------------------------------------------------
*
.MODEL RDRAIN RES (
+TC1 = 0.008891
+TC2 = 3.056e-05)
*
.MODEL RSOURCE RES (
+TC1 = -0.003198
+TC2 = 2.60004e-05)
*
.MODEL RDBODY RES (
+TC1 = 0.003945
+TC2 = 9.54752e-06)
*
*
.MODEL MAIN NMOS (
+LEVEL = 3
+VTO = 3.8
+KP = 13
+GAMMA = 2.6
+PHI = 0.6
+LAMBDA = 0.0019
+RD = 0
+RS = 0
+CBD = 0
+CBS = 0
+IS = 1e-14
+PB = 0.8
+CGSO = 0
+CGDO = 0
+CGBO = 0
+RSH = 0
+CJ = 0
+MJ = 0.5
+CJSW = 0
+MJSW = 0.33
+JS = 1e-14
+TOX = 1e-07
+NSUB = 1e+15
+NSS = 0
+NFS = 6.59e+11
+TPG = 1
+XJ = 0
+LD = 0
+UO = 600
+UCRIT = 1000
+UEXP = 0
+UTRA = 0
+VMAX = 0
+NEFF = 1
+KF = 0
+AF = 1
+FC = 0.5
+DELTA = 0
+THETA = 0
+ETA = 0
+KAPPA = 0.2)
*
*--------------------------------------------------------------------------
*
.MODEL DGD D (
+IS = 1e-15
+RS = 0
+N = 1000
+TT = 0
+CJO = 1.129e-09
+VJ = 1.943
+M = 1.476
+EG = 1.11
+XTI = 3
+KF = 0
+AF = 1
+FC = 0.5
+BV = 10000
+IBV = 0.001)
*
*--------------------------------------------------------------------------
*
.MODEL DBODY D (
+IS = 1.532e-11
+RS = 0
+N = 1.062
+TT = 2.5e-07
+CJO = 9.725e-10
+VJ = 1.127
+M = 0.6627
+EG = 1.11
+XTI = 5
+KF = 0
+AF = 1
+FC = 0.5
+BV = 671
+IBV = 0.00025)
.ENDS

 

[IRstuff]

But what's not supported? Can you move those parameters and related parasitics to be an external component?

TTFN

 

[Maxish]

I should've been slightly more clear. My simulator complains about the actual NMOS SPICE element in the subcircuit. This guy:

.MODEL MAIN NMOS (
+LEVEL = 3
+VTO = 3.8
+KP = 13
+GAMMA = 2.6
+PHI = 0.6
+LAMBDA = 0.0019
+RD = 0
.
.)

It doesn't like lambda amongst a few others at LEVEL 3. Lamda for instance is only supported for LEVEL 1 and 2 as per SPICE manuals.

 

[2dye4]

Max
all those parameters in your nmos model except LAMBDA are
supported in Level 1,2.

Lambda is the channel length modulation parameter.
It will affect the drain to source current with fixed
gate voltage in the saturation region. More lambda makes
a steeper increase in current as Vds increases.

I would enter the formula but there are two many unsupported symbol types.

You can do two things.
change Level back to 1 or remove the lambda value.

In either case build a test circuit in spice after you
change the model and compare the response to data sheet
values. Try to enter a circuit just like the data sheet
and check curves.

 

[2dye4]

Max
Correction
I meant to say all the parameters are supported in level 3
except LAMBDA.

All the parameters listed are included in level 1.
So this really is a level 1 model.
My recommendation is to change level to 1.

Many of the parameters in the higher levels are designed to
account for the tiny geometries in very small mosfets found
on chips. They are not needed for power devices.

 

[Maxish]

no, many are not supported in level 1. The entire set of parameters as they are, cannot be supported by any unmodified SPICE simulator, at any MOSFET level.

Here's a table of which many copies I have seen:

http://www.seas.upenn.edu/~jan/spice/spice.MOSparamlist.html

 

[2dye4]

Sorry
I didn't realize your 17:45 post was an abbreviated
version of your model.

Some of the parameters are Level 2 only.
UCRIT - UEXP - UTRA - NEFF

If you remove CBD and CBS the rest fit into level 2.

Thats about the best I can do.

Good luck