开云体育

PS: It's rumored that most of what the subcircuit models attempt to
do can be done by specifying parameters in the higher-level MOS
models (the "LEVEL=__" parameter) but I haven't found any
documentation or explanation of how to do it.

Dale

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 <
8&oe=UTF-8&group=sci.electronics.cad> and
<
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, )
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!

--- 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, )
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?

Hello ravton,
the provided model is a subcircuit. You can make a symbol like you
would do it for a specific opamp.
Another option is to use a more generalized symbol like my x-models.
I have uploaded these x-models this evening to this group's
files/library menues. There is also a help file there.
Anyway I will send you an example with your model directly.
If you still have problems with it, let me know.

Best Regards
Helmut

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, )
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!

Hello,
I have written a utilty program that makes the LTSpice program
even more useful.

The features are:

1.
Merge as many raw files you want into one raw file.
The advantage is that you can have different simulations in one graph.

2.
Extract data to your spreadsheet or favorite graph program.
You select the signals you want ang get a column based output.

3.
Equalize time steps of .TRAN simulation.
Normally you have never exact the time steps you want in a raw file.
This can become necessary if you want export data to other programs.

These are the most important functions of the program.

If you ever have experienced different simulations in one plot or
easy exporting data to another graphic program, you will be impressed.

I hope that in some future time, all these features are implented in
LTSpice.

Thanks to Mike Engelhardt for the great LTSpice and the support.

Enjoy the program!

Helmut

Helmut Sennewald wrote:

Hello Mike,
sorry for the late response, but I am more in open
newsgroups until now. There I often help people
starting with LTspice.

Hi .. thanks for the reply! Which newsgroup do you suggest?
I only went for the yahoo list because the LTspiceman
pointed me towards it.

If you still have problem with that MAX931 model, then
let me know and I will do it as an example for you.

That's very kind of you, I may take you up on that.
(For now, I've switched to an LT device.)

Mike

--- Mike Cowlishaw <mfcowli@...> schrieb: >
Ralph R. Reinhold wrote:

Mike
It looks like you may have not included a ".lib"

command line in the

schematic.

OK, will investigate ... thanks! Though I think it
is finding the file OK,
because it complained when I had the wrong number of
parameters on the
.subckt statement.

Mike Cowlishaw

Hello Mike,
sorry for the late response, but I am more in open
newsgroups until now. There I often help people
starting with LTspice.

If you still have problem with that MAX931 model, then
let me know and I will do it as an example for you.

Best Regards
Helmut

__________________________________________________________________

Gesendet von Yahoo! Mail -
Weihnachts-Einkufe ohne Stress!

Ralph R. Reinhold wrote:

Mike
It looks like you may have not included a ".lib" command line in the
schematic.

OK, will investigate ... thanks! Though I think it is finding the file OK,
because it complained when I had the wrong number of parameters on the
.subckt statement.

Mike Cowlishaw

Mike
It looks like you may have not included a ".lib" command line in the
schematic. For example,

.lib standard.opamp

.lib dly-line.sub

.lib potentiometer.sub

My guess is that you may need an include statement for this particular
case to call the library.

.include max931.fam

But, I haven't used that command yet.

Ralph



--- In LTspice@y..., "Mike Cowlishaw" <mfcowli@a...> wrote:

Hello,

I'm experimenting with adding a custom model to use in

SwitcherCADiii (I'm

adding a Max931, but with a 'DIP8' symbol and using the Spice model

from

Maxim -- almost the same as an LTC1540). I have the symbol part

working

(Ralph's guide was very useful, I have some experiences to add about

the

semantics of PINs and their ordering if anyone interesting).

I'm now as far as having the model start to run, but just get a

message box:

Spice error
Error: Unknown device type in: xu1 n003 n002 n001 0 n002 n002 out

0

max931.fam max931

(which just looks like the call to the subcircuit with the filename

and

Value added). There's no additional information in the .log file.

Anyone know how I can get more detailed information on the unknown

device

type, or do I just have to plough through the model 'by eye'?

--
Mike Cowlishaw
Coventry, UK

Hello,

I'm experimenting with adding a custom model to use in SwitcherCADiii (I'm
adding a Max931, but with a 'DIP8' symbol and using the Spice model from
Maxim -- almost the same as an LTC1540). I have the symbol part working
(Ralph's guide was very useful, I have some experiences to add about the
semantics of PINs and their ordering if anyone interesting).

I'm now as far as having the model start to run, but just get a message box:

Spice error
Error: Unknown device type in: xu1 n003 n002 n001 0 n002 n002 out 0
max931.fam max931

(which just looks like the call to the subcircuit with the filename and
Value added). There's no additional information in the .log file.

Anyone know how I can get more detailed information on the unknown device
type, or do I just have to plough through the model 'by eye'?

--
Mike Cowlishaw
Coventry, UK

-
You're looking on your computer. Look in the Yahoo Groups.

--- In LTspice@y..., "Ralph R. Reinhold" <rreinhold@a...> wrote:

It is in files under lib then sub. The symbol is under lib then

sym.

I tried to stick to the format of the files loaded with LTSpice.

Ralph where is this potentiometer.
I can't seem to find it.
Thanks,
Keith

Ralph, I still can't seem to find it.
I downloaded the last version of SWCADD.
What is the potentiometer file names.
Also in a post last month you mentioned
something about a TUT folder. I don't have
that folder in my SWCADD file folder as well.
Is there somewhere I could down load this
information.

It is in files under lib then sub. The symbol is under lib then sym.
I tried to stick to the format of the files loaded with LTSpice.

--- In LTspice@y..., "Ralph R. Reinhold" <rreinhold@a...> wrote:

Thanks Larry. It should be fixed now.
Ralph
--- In LTspice@y..., "ve3crx" <ve3crx@r...> wrote:

The potentiometer model in the file area is missing the

subcircuit.

Only the .asy fil is there - in both directories

Larry

Ralph where is this potentiometer.
I can't seem to find it.
Thanks,
Keith

Thanks Larry. It should be fixed now.
Ralph

The potentiometer model in the file area is missing the subcircuit.
Only the .asy fil is there - in both directories

Larry

Mike,
Thank you very much!

Stefano Delfiore

--- Panama Mike <panamatex@...> wrote:

Stefano,

[...]Error: unknown token in: "[!](v(1))"[...]
I have no idea about this error, someone can
give me an help?

It's a spurious error message, and I've implemented
the fix in the source code for the next maintenance
release. In the meanwhile, you can either ignore
the message or or rewrite

b1 3 0 v=!(v(1))

as

b1 3 0 v=inv(v(1))

--Mike

__________________________________________________
Do you Yahoo!?
Faith Hill - Exclusive Performances, Videos & More

__________________________________________________
Do you Yahoo!?
Faith Hill - Exclusive Performances, Videos & More

Stefano,

[...]Error: unknown token in: "[!](v(1))"[...]
I have no idea about this error, someone can
give me an help?

It's a spurious error message, and I've implemented
the fix in the source code for the next maintenance
release. In the meanwhile, you can either ignore
the message or or rewrite

b1 3 0 v=!(v(1))

as

b1 3 0 v=inv(v(1))

--Mike

__________________________________________________
Do you Yahoo!?
Faith Hill - Exclusive Performances, Videos & More

I used a B source to make an inverter gate.
sim
.subckt inv 1 2
b1 3 0 v=!(v(1))
r1 3 2 100
c1 2 0 10P
.ends inv
vin 10 0 pulse 0 10 1m 1n 1n 2m 4m
x1 10 20 inv ic=0
r1 20 0 1meg
.tran 100u 10m 0m 100u
.end

The behavior of the circuit seems to be ok but I got in the "spice
error log" the following message:

Circuit: sim

Error: unknown token in: "[!](v(1))"Date: Sun Oct 13 22:16:06 2002
Total elapsed time: 0.050 seconds.

tnom = 27
temp = 27
method = modified trap
totiter = 792
traniter = 789
equations = 6
tranpoints = 383
accept = 357
rejected = 26
trancuriters = 0


I have no idea about this error, someone can give me an help?
Stefano

I have posted a custom symbols guide in the Files. It is in the 'Tut'
folder.

Thanks to Mike Englehardt for his comments.