Advanced FET Models for LTSpice

[Peter Jacobi]

Dear All!

The Fairchild FET models, e.g. for BSS84, BS138 or
Vishay/Siliconix Si4532ADY use subcircuits instead of
a single MOSFET model.

In LTSpice the 2N7002 works the same, nevertheless I
wasn't able to put the other models to work in LTSpice.

I don't think the problem is with the subcircuit, but
that LTSpice uses older MOSFET models, not Level 3?

But perhaps I goofed when moving the files.

Has anybody insights to offer?

Snippet from the Si4532ADY model:
**************************************************************************
..MODEL NMOS NMOS (LEVEL = 3 TOX = 5E-8
+ RS = 11.5E-3 RD = 0 NSUB = 1.6E17
+ kp = 2.6E-5 UO = 650
+ VMAX = 0 XJ = 5E-7 KAPPA = 12E-2
+ ETA = 1E-4 TPG = 1
+ IS = 0 LD = 0
+ CGSO = 0 CGDO = 0 CGBO = 0
+ NFS = 0.8E12 DELTA = 0.1)
***********************************************************************

Are all these parameters supported by LTSpice?

Regards,
Peter Jacobi

 

[Helmut Sennewald]

----- Original Message -----
From: "Peter Jacobi" <peter_jacobi@gmx.net>
Newsgroups: sci.electronics.cad
Sent: Wednesday, December 17, 2003 1:38 PM
Subject: Advanced FET Models for LTSpice

Dear All!

The Fairchild FET models, e.g. for BSS84, BS138 or
Vishay/Siliconix Si4532ADY use subcircuits instead of
a single MOSFET model.

In LTSpice the 2N7002 works the same, nevertheless I
wasn't able to put the other models to work in LTSpice.

Hello Peter,
you need subcircuit symbols for these devices.
I tried successfully all your mentioned MOSFETS with LTSPICE.

You can find the subcircuit symbols(x-symbols) in the "Files"
section of the LTSPICE-YAHOO-group or you have to make your own symbols.
I recommend to download it. You need also a ".include xxxxx.mod"
command line for every model-file you need in your schematic.
A model file may contain as many models as you like.
The link to the symbols:
http://groups.yahoo.com/group/LTspice/files/lib/sym/Universal%20Subcircuits/
BSS138, n-MOS from the Si4532N -> "xnmos.asy"
p.asy-MOS from the Si4532P -> "xpmos.asy"
BSS84 (4 pins) -> "xpmos4.asy" Connect 1MEG to the 4th
pin.

The plot Id(Vgs) agrees very well with the datsheets for NMOS and PMOS
of the SI4532ADY model, but the simulated current of the BSS84 and the BS138
has been only about 50% of the datasheet Id(Vgs) curve.

Snippet from the Si4532ADY model:
**************************************************************************
.MODEL NMOS NMOS (LEVEL = 3 TOX = 5E-8
+ RS = 11.5E-3 RD = 0 NSUB = 1.6E17
+ kp = 2.6E-5 UO = 650
+ VMAX = 0 XJ = 5E-7 KAPPA = 12E-2
+ ETA = 1E-4 TPG = 1
+ IS = 0 LD = 0
+ CGSO = 0 CGDO = 0 CGBO = 0
+ NFS = 0.8E12 DELTA = 0.1)
***********************************************************************

This is the error(warning) message from LTSPICE:
------------------------------------------------
Error on line 76 : .model §u1:nmos nmos (level = 3 tox = 5e-8 rs = 11.5e-3
rd = 0 nsub = 1.6e17 kp = 2.6e-5 uo = 650 vmax = 0 xj = 5e-7 kappa =
12e-2
eta = 1e-4 tpg = 1 is = 0 ld = 0 cgso = 0 cgdo = 0 cgbo = 0 tlev = 1
bex = -1.5 tcv = 3.75e-3 nfs = 0.8e12 delta = 0.1)
Unrecognized parameter "tlev" - ignored
Unrecognized parameter "bex" - ignored
Unrecognized parameter "tcv" - ignored

I don't think the problem is with the subcircuit, but
that LTSpice uses older MOSFET models, not Level 3?

But perhaps I goofed when moving the files.

Has anybody insights to offer?

I hope that Mike Engelhardt will answer your question about the ignored
parameters.
At least the simulated Id(Vgs) agrees very well with the datasheet.

Best Regards,
Helmut

 

[Mike Engelhardt]

Helmut,

This is the error(warning) message from LTSPICE:

Error on line 76 : .model §u1:nmos nmos (level = 3
tox = 5e-8 rs = 11.5e-3 rd = 0 nsub = 1.6e17
kp = 2.6e-5 uo = 650 vmax = 0 xj = 5e-7 kappa = 12e-2
eta = 1e-4 tpg = 1 is = 0 ld = 0 cgso = 0 cgdo = 0
cgbo = 0 tlev = 1 bex = -1.5 tcv = 3.75e-3
nfs = 0.8e12 delta = 0.1)
Unrecognized parameter "tlev" - ignored
Unrecognized parameter "bex" - ignored
Unrecognized parameter "tcv" - ignored

Thanks, Helmut for pointing out there remained a
question outstanding here. tlev, bex, and tcv
aren't level 3 MOSFET parameters. PSpice ignores
them and doesn't do anything with them. LTspice has
different parsers for every MOSFET level, so it knows
when you're using a parameter that doesn't belong.
PSpice doesn't complain about using a parameter that
doesn't apply to that level. You'll find lots of models
with this type of unimportant error in the public domain
because they where "checked" in PSpice that didn't
check for this type of error in the way the model was
written.

--Mike