Quick Hints (Check this post carefully; NOT GUARANTEED ERROR FREE):
(Wife is waiting in parking lot to tell me her NEXT husband will
always leave work on time . . . )
The On Semi file is a SUBCIRCUIT model (of a MOSFET, plus some
corrections for its non-idealness as well as package parasitics, etc)
while the "STANDARD.MOS" file is a database of parameters for MOS
DEVICE models. It's certainly confusing and perhaps unfortunate that
MOSFETS (in particular) are commonly modeled by both methods, but
that's how it is. What REALLY tripped you up is when the subcircuit
model builder chose to call a resistor "Rg" which is the same name as
a parameter in the MOS device model. (He should have stuck with
something like "R101" and let us guess what it's role is.)
You probably want to copy the On Semi file to the " .\LIB\SUB\"
directory and call it something like "ntmd6p02r2.sub". (If you have
a bunch of these files, you might creat a sub-directory
called ".\LIB\SUB\ON_SEMI\" to hold them; or concatenate them into a
largeer file called "ON_SEMI_MOSFET.LIB")
Next make a symbol file that references this model, perhaps
called ".\lib\sym\PowerMOS\ntmd6p02r2.asy". Do this with the symbol
editor in LTSpice, or copy the following:
Version 3
SymbolType CELL
LINE Normal 12 12 12 24
LINE Normal 4 20 12 20
LINE Normal 4 12 6 12
LINE Normal 12 12 6 11
LINE Normal 12 12 6 13
LINE Normal 6 11 6 13
LINE Normal 4 2 4 6
LINE Normal 4 10 4 14
LINE Normal 4 18 4 22
LINE Normal 0 20 2 20
LINE Normal 2 4 2 20
LINE Normal 12 4 4 4
LINE Normal 12 0 12 4
WINDOW 0 14 8 Left 0
WINDOW 3 14 18 Left 0
SYMATTR Prefix MP
SYMATTR SpiceModel NTMD6P02R2.SUB
SYMATTR Value NTMD6P02R2
SYMATTR SpiceLine *
SYMATTR SpiceLine2 *
SYMATTR Description P-MOSFET 20V, 6A
PIN 0 20 NONE 0
PINATTR PinName G
PINATTR SpiceOrder 2
PIN 12 0 NONE 0
PINATTR PinName D
PINATTR SpiceOrder 1
PIN 12 24 NONE 0
PINATTR PinName S
PINATTR SpiceOrder 3
Close and re-start LTSpice. You should be able to find the symbol
you just created in the component selection menu, and it should point
to your subcircuit model file when you simulate.
(You can probably figure out most of this by poking around in the
LTSpice "HELP" files for a while, but it's not explained very
clearly. Note that both the model file and the symbol file are
straight ASCII and can be attacked with your favorite text editor,
but you'll have to re-start LTSpice to pick up the changes so you
might as well use the LTSpice editor.
The newsgroups at <
http://groups.google.com/groups?hl=en&lr=&ie=UTF-8&oe=UTF-8&group=sci.electronics.cad> and
<
http://groups.google.com/groups?hl=en&lr=&ie=UTF-8&oe=UTF-8&group=sci.electronics.design> are good sources of info on LTSpice:
Mike Englehardt (author of LTSpice) checks them regularly. Search
them with "LTSpice" as a keyword & you'll probably find a discussion
on this very question!)
Dale
--- In LTspice@..., "ravton <ravton@y...>" <ravton@y...>
wrote:
I've only been using LTSpice for a couple of weeks and have finally
gotten stuck. I'm trying to import some additional MOSFET models
(for example, http://www.onsemi.com/pub/Collateral/NTMD6P02R2.LIB )
and am at a loss on how to do it.
I've waded through the online manuals and googled forever. I tried
just copying values from the PSpice model into the standard.mos
file but it's not clear what to copy.
For example, in standard.mos the first parameter is "Rg". The
manual states that "Rg" is "Gate ohmic resistance". But in the
PSPice model the only line with Rg is "RG 2 7 10.013". Now since
every other line in the standard.mos file has Rg=3 I'm totally
confused on how to proceed.
Can anyone provide any hints of guidance on how to import these?
Thanks!
Mike Engelhardt