开云体育

--- In LTspice@..., Panama Mike <panamatex@y...> wrote:

Dale wrote:

Mike, this sounds like something I'd like to
dissuade you from.

Helmult wrote:
I fully agree with you. The biggest advantage
of all the opamp models
[...]
The provided SPICE models should be also optimized
for good convergence in the simulation. If a model
doesn't provide some features like noise modeling
(.AC), it should behave more like an ideal
component in such a type of simulation.

The problem is that the PSpice models often don't
converge very well and don't model noise correctly.
That has nothing to do with Linear's opamp models,
it's common to most Boyle style models.

Hello Mike,
I have never said here that it is specific for LT models. My
statement has been a general one for all vendor's models.
If it is true that the Boyle model is so weak, why not starting with
another SPICE model? I am shure that LT has the right people(you for
example) to make excellent models.

They don't
converge well in PSpice either. It's just a really
lame modeling methodology. Sometimes I honestly
get the impression that SPICE macromodeling
engineers tweak a model until it doesn't run anymore
and pronounce it done at that point, blaming any
convergence problems are due to the simulator.

I have experimented with my own generic opamp model and indeed it
converges very different depending on the choosen circuit.

LTSPICE has been greatly improved over the last year regarding
convergence problems. Most of the problems seem to be history.

Of course the advantage of being able to run
them in PSpice is important.

There are even more SPICE simulators around. Some of them are
specific SPICE simulators like ICAP and others are part of PCB-CAD
packages. All these users need/want SPICE models of LT opamps.
Finally I hope that LT always provide opamp models for the whole
SPICE "family" too.

Best Regards
Helmut

Dale wrote:

Mike, this sounds like something I'd like to
dissuade you from.

Helmult wrote:
I fully agree with you. The biggest advantage
of all the opamp models
[...]
The provided SPICE models should be also optimized
for good convergence in the simulation. If a model
doesn't provide some features like noise modeling
(.AC), it should behave more like an ideal
component in such a type of simulation.

The problem is that the PSpice models often don't
converge very well and don't model noise correctly.
That has nothing to do with Linear's opamp models,
it's common to most Boyle style models. They don't
converge well in PSpice either. It's just a really
lame modeling methodology. Sometimes I honestly
get the impression that SPICE macromodeling
engineers tweak a model until it doesn't run anymore
and pronounce it done at that point, blaming any
convergence problems are due to the simulator.

Essentially all customer-reported SwCADIII
convergence problems reported deal with using
these opamp models. But inside the mixed-mode
simulator in LTspice is the ability to model
an opamp model like I described. Few convergence
problems, one or two internal nodes, good noise
modeling and almost no load on the simulation
run time. The technology already exists in
LTspice and is used in the SMPS products' error
amps.

Another problem I have is there's some newer
Linear opamps that don't have any SPICE models.
If I go to this new method, then I can make a
model in less than an hour that will be more
accurate than the former PSpice models. It's
much cheaper and it's hard to justify these
expensive PSpice models that don't work well.
Of course the advantage of being able to run
them in PSpice is important.

--Mike

__________________________________________________
Do you Yahoo!?
Yahoo! Platinum - Watch CBS' NCAA March Madness, live on your desktop!

--- In LTspice@..., "Dale" <dchishol@c...> wrote:

--- In LTspice@..., Message 141, Panama Mike
<panamatex@y...> wrote:
< snip >

BTW, I'm thinking of introducing opamp models that
use a different modeling methodology, similar to
that used for LTspice's SMPS products. The result
would be computationally extremely lightweight and
robust models that model noise too(these PSpice-
style opamp models almost never get the noise
modeled). However, the opamps models would not
run in other SPICE simulators and non-LT opamp
models wouldn't be available. Would you folks be
interested in something like that?

--Mike

Mike, this sounds like something I'd like to dissuade you from.

Part of the strength of the SPICE methodology is that the models are
transmitted as "open source", simple text files. The most

significant

advantage is that we Mere Mortals can easily extend, improve,

correct,

or modify models as needed.

Hello Dale,
I fully agree with you. The biggest advantage of all the opamp models
from different vendors is that they follow the general accepted SPICE
syntax. This standard has been the base for the success of SPICE over
the last thirty years. This is at least true for most of the analog
parts like diodes, transistors, passive components and the opamps.

It may be different for SMPS, because they are much more mixed signal
devices. Here we have a lack of standard for digital parts and also a
missing standard for behavioral language syntax. One more reason is
the needed compuational speed of SMPS models for effective usage. I
believe it is ok to have special models for the SMPS, because they
are developed independently of the other anaolg/digital circuits of a
design.

Hello Mike,
I recommend to keep the "easier" parts like opamps compatible with
standard (P)SPICE, because many of LT customers use other SPICE
simulators for different reasons.
The provided SPICE models should be also optimized for good
convergence in the simulation. If a model doesn't provide some
features like noise modeling (.AC), it should behave more like an
ideal component in such a type of simulation.

Best Rgeards
Helmut

--- In LTspice@..., Message 141, Panama Mike
<panamatex@y...> wrote:
< snip >

BTW, I'm thinking of introducing opamp models that
use a different modeling methodology, similar to
that used for LTspice's SMPS products. The result
would be computationally extremely lightweight and
robust models that model noise too(these PSpice-
style opamp models almost never get the noise
modeled). However, the opamps models would not
run in other SPICE simulators and non-LT opamp
models wouldn't be available. Would you folks be
interested in something like that?

--Mike

Mike, this sounds like something I'd like to dissuade you from.

Part of the strength of the SPICE methodology is that the models are
transmitted as "open source", simple text files. The most significant
advantage is that we Mere Mortals can easily extend, improve, correct,
or modify models as needed.

The parent thread for this posting is a good example. Because almost
everything about the model was in plain view, several minds were
independently analyzing the problem and solving it. I cannot imagine
the problem being resolved nearly as quickly if the model's topology
and parameter values had been locked-up in a proprietary format
readable only by a few people.

The SPICE methodology permits individuals to customize models as
needed. If, for instance, noise is a critical performance
characteristic the necessary elements can be readily included to model
it. Otherwise they may be omitted. Similarly, a small-signal stage
where output limiting is not a concern can get by with a simplified
output circuit in the model.

Along the same line it is relatively easy to adjust model parameters
to fit particular situations. The model can be customized to reflect
the device's behavior at, say, a temperature extreme. Or an engineer
can investigate the implications of using a device whose performance
parameters (like offset voltage or slew rate) are near the data sheet
limits. Likewise the need for parts specially selected for certain
characteristics (such as low offset current) can be evaluated.

Finally the current SPICE modeling methodology allows engineers to
quickly create workable models for new or alternative components.

I hope that whatever modeling methodology you choose will retain these
features.

Dale

Quite apart from LTSpice, please accept a moral and ethical
commendation. By living in another culture & learning its language
you are promoting international understanding and respect for all
persons. This is unusual even among educated professionals. When I
was rushed to Mexico City after the earthquake, I learned that one of
my co-workers believed ANYBODY could understand English if only it was
spoken loudly and clearly enough.

An old joke asks, "If somebody who speaks 3 languages is trilingual
and somebody who speaks 2 languages is bilingual, what term describes
somebody who speaks but one language?" The answer, of course, is
"American". This situation is a symptom of a larger arrogance and
self-centeredness which we never intended to cultivate and are
certainly not proud of, but which often limits our ability to accept
others as truly human and our equals. (Yes, I include myself in that
indictment: with the minimal Spanish I learned in High School I could
bumble through ordering from a menu, and possibly even ask for
directions, but writing a coherent paragraph, reading a newspaper or
even normal conversation are beyond me. )

Again, thanks for doing your part. I hope nobody recognizes that I
carry a Scottish name and expects me to reply in Gaelic . . .

--- In LTspice@..., Arnold Esper <arnold.esper@n...>
wrote:

Hallo Helmut and Mike Engelhardt,

thanks for finding and solving the +problem. My (LTspice-)World

doesn't seem to

collapse in the near future any more.

Hello Arnold and all LTSPICE users.
I have uploaded an example how your netlist based circuit can be
converted to a LTSPICE schematic and model file. It is hopefully all
explained in the comments in this schematic. All the necessary files
are in the files area of this group.

Files->Examples->Educational->From netlist to schematic

Have fun with it.

Thanks to Mike too for the correction of the '+' problem in the PWL
syntax.

Best Regards
Helmut

Arnold,

thanks for finding and solving the +problem.
My (LTspice-) World doesn't seem to collapse
in the near future any more.

Das freut mich. (English: Glad to hear it.)

Mr. Engelhardt, are you German? your Name is.

Nee, ich bin Amerikaner. Aber ich wohnte ein
Jahr in Mainz. Nicht bei der Army aber auf
der Uni. Das war in 1978. Man versteht meine
deutsch Errantnisse ist in der Zwichenseit
auseinander gefallen. Normaleweise versuche
ich nie auf deutsch zu schreiben.

(English: Nope, I'm American. But I lived
a year in Mainz, Germany. Not with the Army
but at the university. That was in 1978
and my German knowledge has fallen to pieces
in the meanwhile. Normally I avoid writing
in German Language.)

--Mike

__________________________________________________
Do you Yahoo!?
Yahoo! Platinum - Watch CBS' NCAA March Madness, live on your desktop!

Hallo Helmut and Mike Engelhardt,

thanks for finding and solving the +problem. My (LTspice-)World doesn't seem to
collapse in the near future any more.

Mr. Engelhardt, are you German? your Name is.

Arnold

Helmut,

Would it be difficult to improve your
interpreter so that it correctly
accepts a '+' sign?

OK. What's happening is that the
'+' sign can be used to mean incremented
from the previous value. It's a PSpice
convention useful for time points as in

V2 1 0 PWL (0 0 +1m 1 +1m 0 +1m 1 +1m 0 +1m 1)

But I'll turn that off for the voltage
in a future version, since I don't think
it should do it for the voltage, just the
time.

The web has just been updated with a
version that doesn't interpret the '+'
sign as incremental from the previous
version for voltage but still does for
time.

Thanks for pointing out the problem.

--Mike

__________________________________________________
Do you Yahoo!?
Yahoo! Platinum - Watch CBS' NCAA March Madness, live on your desktop!

Helmut,

Would it be difficult to improve your
interpreter so that it correctly
accepts a '+' sign?

OK. What's happening is that the
'+' sign can be used to mean incremented
from the previous value. It's a PSpice
convention useful for time points as in

V2 1 0 PWL (0 0 +1m 1 +1m 0 +1m 1 +1m 0 +1m 1)

But I'll turn that off for the voltage
in a future version, since I don't think
it should do it for the voltage, just the
time.

--Mike

__________________________________________________
Do you Yahoo!?
Yahoo! Platinum - Watch CBS' NCAA March Madness, live on your desktop!

--- In LTspice@..., Arnold Esper <arnold.esper@n...>
wrote:

Guten Tag,
was sind das für Fehler in LT-Spice? Gerechnet mit LT-Spice und

Winspice3.

Hallo Arnold,
hier kann fast keiner deutsch, deshalb macht es wenig Sinn die Frage
zus?tzlich in deutsch zu stellen.

what sort of errors is this in LT-Spice? The Schematic is computed

with LT-Spice

and Winspice3 from Mike Smith.
V1 1 0 DC 0 AC 1 PWL(0 0V 1m 0V 5m -.6V 13m +.8V 17m 0V)

I had the same problem some times ago with a model I think. The
problem here is that LTSPICE cannot interpret the '+' sign of a
number. So simply remove the '+' at the beginning of any number.
V1 1 0 DC 0 AC 1 PWL(0 0V 1m 0V 5m -.6V 13m .8V 17m 0V)

WINSPICE and PSPICE! have no problem with the '+' sign.

I didn't find any control to max Time Steps in
the .trans analysis.
.TRAN 10u 20m

You have to give four parameters if you want specify a maximum time
step. The command line could look in your example like this one.
.TRAN 10u 20m 0 10u
The other chance is a .option command line.
.TRAN 20m
.OPTIONS maxstep=10u


Hello Mike,
would it be difficult to improve your interpreter so that it
correctly accepts a '+' sign?

Best Regards
Helmut

Guten Tag,
was sind das fr Fehler in LT-Spice? Gerechnet mit LT-Spice und Winspice3.

Hello,
what sort of errors is this in LT-Spice? The Schematic is computed with LT-Spice
and Winspice3 from Mike Smith. I didn't find any control to max Time Steps in
the .trans analysis.

Arnold


BEGRE00 Begrenzer mit Transistoren


* *
* B E G R E N Z E R T R A N S I S T O R E N 0 0 . C I R *
* *
* Begrenzer mit Transistoren und Dioden in der Gegenkopplung *
* Benutzter OPA: TL 051 *
* *
* 20.03.2003 Arnold Esper *
* *



* *
* Definition der Eingangsspannung VIN zwischen Knoten 1 und 0 mit AC *
* und Puls, AC mit 1VOLT, der Puls wird festgelegt durch : *
* *
* PULS(U1 U2 T_VERZOEGER T_ANSTIEG T_ABFALL T_WEITE T_PERIODE) *
* *
* U2_|_ _ ______________ ____ *
* | / &#92; / *
* | / &#92; / *
* | / &#92; / *
* U1-|-------- - - - - - ------------------------ *
* | *
* *
* T_VERZ |T_AN| T_WEITE |T_AB| *
* | T_PERIODE | *
* *

* *
* Definition einer Polygonquelle (piece-wise-linear) *
* *
* PULS(U1 U2 T_VERZOEGER T_ANSTIEG T_ABFALL T_WEITE T_PERIODE) *
* *
* _|_ ______________ *
* | / &#92; *
* | / &#92; *
* | / &#92; *
* u0-|------- - - - - - &#92;- - - - - - - - - - *
* | &#92; *
* | &#92;____________________________ *
* *
* | | | | | *
* t0 u0 t1 u1 t2 u2 t3 u3 t4 u4 *
* *


*V1 1 0 DC 0 AC 1 PULSE(0 .6 100u 1m 1m 1n 1s)

**** Polygon-Quelle **

V1 1 0 DC 0 AC 1 PWL(0 0 1m 0V 5m -.6V 13m +.8V 17m 0V)



R1 1 2 22K
R2 2 4 22K
R3 4 6 100K
R4 6 7 22K
D1 2 3 DI
D2 7 5 DI
Q1 3 6 7 BC550C
Q2 5 4 2 BC550C
*E0 7 0 0 2 100K
X1 0 2 60 70 7 TL051/TI

* Betriebsspannungen VP VN ***

VP 60 0 DC 15
VN 70 0 DC -15

**** Analysen ****

*.OPTIONS LIMPTS=10000
*.AC DEC 100 10 20000
*.PRINT AC VDB(7)
.TRAN 10u 20m
.PRINT TRAN V(7)
*.DC V1 -1 1 0.001
*.PRINT DC V(7)


.model DI D



.model BC550C NPN(Is=7.049f Xti=3 Eg=1.11 Vaf=23.89 Bf=493.2 Ise=99.2f
+ Ne=1.829 Ikf=.1542 Xtb=1.5 Br=2.886 Isc=7.371p
+ Nc=1.508 Ikr=5.426 Rc=1.175 Cjc=5.5p Mjc=.3132 Vjc=.4924 Fc=.5
+ Cje=11.5p Mje=.6558 Vje=.5 Tr=10n Tf=420.3p Itf=1.374 Xtf=39.42
+ Vtf=10)
* PHILIPS pid=bc549c case=TO92
* 91-07-31 dsq

*
* TL051 operational amplifier "macromodel" subcircuit
* created using Parts release 4.01 on 04/12/89 at 09:57
* (REV N/A)
* connections: non-inverting input
* | inverting input
* | | positive power supply
* | | | negative power supply
* | | | | output
* | | | | |
.subckt TL051/TI 1 2 3 4 5
*
c1 11 12 3.988E-12
c2 6 7 15.00E-12
dc 5 53 dx
de 54 5 dx
dlp 90 91 dx
dln 92 90 dx
dp 4 3 dx
egnd 99 0 poly(2) (3,0) (4,0) 0 .5 .5
fb 7 99 poly(5) vb vc ve vlp vln 0 2.875E6 -3E6 3E6 3E6 -3E6
ga 6 0 11 12 292.2E-6
gcm 0 6 10 99 6.542E-9
iss 3 10 dc 300.0E-6
hlim 90 0 vlim 1K
j1 11 2 10 jx
j2 12 1 10 jx
r2 6 9 100.0E3
rd1 4 11 3.422E3
rd2 4 12 3.422E3
ro1 8 5 125
ro2 7 99 125
rp 3 4 11.11E3
rss 10 99 666.7E3
vb 9 0 dc 0
vc 3 53 dc 3
ve 54 4 dc 3.700
vlim 7 8 dc 0
vlp 91 0 dc 28
vln 0 92 dc 28
.model dx D(Is=800.0E-18)
.model jx PJF(Is=15.00E-12 Beta=185.2E-6 Vto=-1)
.ends

*

.END

Sean,

See the examples called wavein.asc and waveout.asc in
the "educational" folder and also see help files for .wave

It is very cool indeed!

Brad


--- In LTspice@..., "sean_schouten" <sean_schouten@y...>
wrote:

Hi!

I too am new to spice. I heard that you were supposed to export a
output-waveform to a Wav-file somehow. Can any-one tell me how?

Would be cool.

Cheers, Sean

Hi!

I too am new to spice. I heard that you were supposed to export a
output-waveform to a Wav-file somehow. Can any-one tell me how?

Would be cool.

Cheers, Sean

Steve,

[...]Is this a fluke? Is there any way to tell if
a model will predict noise performance in general
and 1/f noise in particular.

I'm afraid it probably was, unless noise was
dominated by the resistors of your circuit.
Noise doesn't appear to be modeled in the LT2018A
macro model.

I think the only opamp macro model that claims to
model noise is the LT1028N.

--Mike

__________________________________________________
Do you Yahoo!?
Yahoo! Platinum - Watch CBS' NCAA March Madness, live on your desktop!

Thanks for the help on the Burr Brown amp.

Noise analysis is a nice feature of LTSpice. It's helpful to poke
around a circuit to see where noise is being generated. However, I
didn't put alot of credence into the actual predictions because of
potential limitations in the SPICE models.

Out of curosity, I compared the RMS noise in an actual circuit using
a couple of different op amps, including the LT2078A. I found that
the predicted noise was fairly close to the actual measured values.
The circuit is basically DC-coupled so 1/f noise is expected to be
significant.

Is this a fluke? Is there any way to tell if a model will predict
noise performance in general and 1/f noise in particular.

Steve H.

thanks Helmut, its running ok with models downloaded
from duncanamps.com
thanks a lot

guille

--- Helmut Sennewald <helmutsennewald@...>
wrote:

--- In LTspice@..., Bill Lewis
<wrljet@y...> wrote:

Please post any replies to this question to the

list.

I'm interested in vacuum tube modeling.

... and the obvious question: How do I relate the

previous info
with

the symbol.

Hello Bill,
you will find the symbol in the "misc" directory.
A short description follows:
1. Load the triode symbol into your schematic.
2. Replace the value 'triode' with the model name
used in the model
file. In this case it is '12AX7A'.
3. Put the model text into a file and store it in
your working
directory. That is the directory where your
schematic is.
4. Add the line .INCLUDE modelfilename in your
schematic.
That's it. This procedure will work for any kind of
part and you can
put as many models you want into one file.

It is important for any kind of symbol and model
that the pin order
is matching. Let's take a look to the triode symbol.
The provided
symbol has the pin order P(1), G(2), K(3). The model
text
uses .SUBCKT 12AX7A P G K . This means that P
is pin-1 G is pin-
2 and K is pin-3. We have luck, the pin order is the
same. If it is
different, then we could either change the order in
the model text or
in the symbol.

I have the ready to run example files attached.

By the way, the model isn't good at low Vpk
voltages. Take a look to
the Ip(Vgk, Vpk) plot to see what I mean.

Best Regards
Helmut




The model file: triode_12ax7a.sub
---------------------------------

* 12AX7A Triode PSpice Model 8/96, Rev. 1.0 (fp)
*
*

-------------------------------------------------------------------

* This model is provided "as is", with no warranty
of any kind,
* either expressed or implied, about the suitability
or fitness
* of this model for any particular purpose. Use of
this model
* shall be entirely at the user's own risk.
*
* For a discussion about vacuum tube modeling please
refer to:
* W. Marshall Leach, jr: "SPICE Models for
Vacuum-Tube Amplifiers";
* J. Audio Eng. Soc., Vol 43, No 3, March 1995.
*

-------------------------------------------------------------------

*
* This model is valid for the following tubes:
* 12AX7A/ECC83, 7025, 6EU7, 6681, 6AV6, 12DW7/7247
(Unit #1);
* at the following conditions:
* Plate voltage : 25..400V
* Grid voltage : 0..-3.5V
* Cathode current: 0..8mA
*
*
* Connections: Plate
* | Grid
* | | Cathode
* | | |
.SUBCKT 12AX7A P G K
E1 2 0 VALUE={45+V(P,K)+95.43*V(G,K)}
R1 2 0 1.0K
Gp P K
VALUE={1.147E-6*(PWR(V(2),1.5)+PWRS(V(2),1.5))/2}
Cgk G K 1.6P
Cgp G P 1.7P
Cpk P K 0.46P
.ENDS 12AX7A.SUBCKT 12AX7A P G K


The circuit file: triode_test.asc
---------------------------------

Version 4
SHEET 1 1104 692
WIRE 336 384 336 496
WIRE 368 288 368 224
WIRE 368 224 512 224
WIRE 512 336 512 224
WIRE 512 416 512 496
WIRE 512 496 336 496
WIRE 336 496 176 496
WIRE 176 496 176 448
WIRE 176 368 176 336
WIRE 176 336 320 336
WIRE 176 528 176 496
FLAG 176 528 0
SYMBOL F:&#92;PROGRAMME&#92;LTC&#92;SWCADIII&#92;lib&#92;sym&#92;Misc&#92;triode
368 336 R0
SYMATTR InstName U1
SYMATTR Value 12AX7A
SYMBOL F:&#92;PROGRAMME&#92;LTC&#92;SWCADIII&#92;lib&#92;sym&#92;voltage 176
352 R0
WINDOW 123 0 0 Left 0
WINDOW 39 0 0 Left 0
SYMATTR InstName V1
SYMATTR Value 0
SYMBOL F:&#92;PROGRAMME&#92;LTC&#92;SWCADIII&#92;lib&#92;sym&#92;voltage 512
320 R0
SYMATTR InstName V2
SYMATTR Value 200V
TEXT 142 136 Left 0 !;dc V2 0 200 0.1 V1 -5 20 5
TEXT 136 176 Left 0 !.INCLUDE triode_12ax7a.sub
TEXT 592 136 Left 0 ;.dc V2 0 200 0.1 V1 -5 20 5
Ip(Vpk, Vgk)
TEXT 144 96 Left 0 !.dc V1 -5 20 0.1
TEXT 592 96 Left 0 ;.dc V1 -5 20 0.1
Ip(Vgk)

__________________________________________________
Do you Yahoo!?
Yahoo! Platinum - Watch CBS' NCAA March Madness, live on your desktop!

Reinier,

Sounds interesting. Could you also
make a very simple opamp with the
output voltage limited to the
supply voltages? I sometimes get
Mega Volts in my circuit on 1 Volt
transients at the inputs.

Yes, the thing I have in mind would do
that. Below is a list prepared for
someone else who asked about this
offline:

I've in mind to model GBW, AOL, slew
limit, voltage and current noise and
corner frequencies for each(But not
model noise from input impedance
imbalance like from JFET input
products), dynamic current draw from
each rail, output voltage range,
output current limit, and input bias
current. That can all be modeled in
the modeling methodology used in the
SMPS products one one internal node.
Doing the real small signal transfer
above the dominate pole requires
more nodes. For example, the LT1028
can be done with two more nodes.
CMRR would not be particularly
modeled, but it would be non-zero.

--Mike

__________________________________________________
Do you Yahoo!?
Yahoo! Platinum - Watch CBS' NCAA March Madness, live on your desktop!

--- In LTspice@..., "Helmut Sennewald"
<helmutsennewald@y...> wrote:

--- In LTspice@..., "kaplounovski" <kaplounovski@y...>
wrote:

--- In LTspice@..., Jim Stockton <mstech@p...> wrote:

kaplounovski wrote:

Hello,
I'm trying to use the National LMC6484A opamp model in

LTSpice.

I've downloaded their model and placed it
into ..&#92;LTC&#92;SWCADIII&#92;lib&#92;sub directory under the name

LMC6484A.sub.

Then I created a simple test schematic where I used opamp2

symbol

with

Prefix = X, Spice Model = LMC6484A.sub, Value = LMC6484A.sub
properties.
I've also added the .inc LMC6484A.sub directive to the

netlist.

Running the simulation produces the following error message:
Error: Unknown subckt called in: xu1 ...... lmc6484a.sub lmc

6484a.sub

What am I doing wrong?

Thanks,
Eugene.


To unsubscribe from this group, send an email to:
LTspice-unsubscribe@...



Your use of Yahoo! Groups is subject to

Try leaving model blank and using value = lmc6484a without

the .sub

Good Luck
Jim Stockton

Thank you, Jim.
I tried that, with the same outcome. This is how it was done in

the

old DOS-based PSpice, it worked there. I'm almost sure it's

something

really simple, like missing path or something, but what? Could it

be

that the op-amp's subcircuit in turn includes some models, namely
MOSFET, that LTSpice could not find?
Regards,
Eugene

Hello Eugene,
this is one of the two chances to include your moddel.
You can see the other one in the thread about the OPA336.
Sorry for my short explanations. I must immediately leave my home

to

go work.

Put the symbol file into the LTSPICE lib&#92;sym&#92;opamp directory.
Put the model file National.lib into LTSPICE lib&#92;sub directory.

Best Regards
Helmut


Test circuit file

Version 4
SHEET 1 1372 1316
WIRE 320 320 320 352
WIRE 320 256 320 224
WIRE -16 368 -16 304
WIRE -16 96 80 96
WIRE 80 304 -16 304
WIRE 160 304 240 304
WIRE 160 96 240 96
WIRE 288 272 240 272
WIRE 240 272 240 96
WIRE 464 96 512 96
WIRE 512 96 512 288
WIRE 512 288 352 288
WIRE -16 480 -16 448
WIRE 240 480 240 512
WIRE 384 480 384 512
WIRE 240 592 240 624
WIRE 384 592 384 624
WIRE 512 288 544 288
WIRE 240 96 384 96
WIRE 240 304 288 304
WIRE 320 976 320 1008
WIRE 320 912 320 880
WIRE -16 752 96 752
WIRE 80 960 -16 960
WIRE 160 960 240 960
WIRE 160 752 240 752
WIRE 288 928 240 928
WIRE 240 928 240 752
WIRE 464 752 512 752
WIRE 512 752 512 944
WIRE 512 944 352 944
WIRE 512 944 544 944
WIRE 240 752 384 752
WIRE 240 960 288 960
WIRE -16 1024 -16 960
WIRE -16 1136 -16 1104
FLAG 320 224 Vcc
FLAG 240 480 Vcc
FLAG 384 480 Vss
FLAG 320 352 Vss
FLAG -16 480 0
FLAG 240 624 0
FLAG 384 624 0
FLAG 544 288 out
FLAG 240 96 in-
FLAG 240 304 in+
FLAG -16 96 0
FLAG 320 880 Vcc
FLAG 320 1008 Vss
FLAG 544 944 out1
FLAG 240 752 in1-
FLAG 240 960 in1+
FLAG -16 752 0
FLAG -16 304 in
FLAG -16 1136 0
SYMBOL F:&#92;PROGRAMME&#92;LTC&#92;SWCADIII&#92;lib&#92;sym&#92;voltage 240 496 R0
SYMATTR InstName V1
SYMATTR Value 5
SYMBOL F:&#92;PROGRAMME&#92;LTC&#92;SWCADIII&#92;lib&#92;sym&#92;voltage 384 496 R0
SYMATTR InstName V2
SYMATTR Value -5
SYMBOL F:&#92;PROGRAMME&#92;LTC&#92;SWCADIII&#92;lib&#92;sym&#92;voltage -16 352 R0
WINDOW 123 24 132 Left 0
WINDOW 39 0 0 Left 0
SYMATTR Value2 AC 1
SYMATTR InstName V3
SYMATTR Value 1
SYMBOL F:&#92;PROGRAMME&#92;LTC&#92;SWCADIII&#92;lib&#92;sym&#92;res 368 112 R270
WINDOW 0 32 56 VTop 0
WINDOW 3 0 56 VBottom 0
SYMATTR InstName R1
SYMATTR Value 1MEG
SYMBOL F:&#92;PROGRAMME&#92;LTC&#92;SWCADIII&#92;lib&#92;sym&#92;res 64 320 R270
WINDOW 0 32 56 VTop 0
WINDOW 3 0 56 VBottom 0
SYMATTR InstName R2
SYMATTR Value 1MEG
SYMBOL F:&#92;PROGRAMME&#92;LTC&#92;SWCADIII&#92;lib&#92;sym&#92;res 64 112 R270
WINDOW 0 32 56 VTop 0
WINDOW 3 0 56 VBottom 0
SYMATTR InstName R3
SYMATTR Value 1MEG
SYMBOL F:&#92;PROGRAMME&#92;LTC&#92;SWCADIII&#92;lib&#92;sym&#92;res 368 768 R270
WINDOW 0 32 56 VTop 0
WINDOW 3 0 56 VBottom 0
SYMATTR InstName R4
SYMATTR Value 1MEG
SYMBOL F:&#92;PROGRAMME&#92;LTC&#92;SWCADIII&#92;lib&#92;sym&#92;res 64 976 R270
WINDOW 0 32 56 VTop 0
WINDOW 3 0 56 VBottom 0
SYMATTR InstName R5
SYMATTR Value 1
SYMBOL F:&#92;PROGRAMME&#92;LTC&#92;SWCADIII&#92;lib&#92;sym&#92;cap 96 768 R270
WINDOW 0 32 32 VTop 0
WINDOW 3 0 32 VBottom 0
SYMATTR InstName C1
SYMATTR Value 1
SYMBOL F:&#92;PROGRAMME&#92;LTC&#92;SWCADIII&#92;lib&#92;sym&#92;voltage -16 1008 R0
WINDOW 123 24 132 Left 0
WINDOW 39 0 0 Left 0
SYMATTR Value2 AC 1
SYMATTR InstName V4
SYMATTR Value 0
SYMBOL F:&#92;PROGRAMME&#92;LTC&#92;SWCADIII&#92;lib&#92;sym&#92;Opamps&#92;LMC6484A 320 224 R0
SYMATTR InstName U1
SYMBOL F:&#92;PROGRAMME&#92;LTC&#92;SWCADIII&#92;lib&#92;sym&#92;Opamps&#92;LMC6484A 320 880 R0
SYMATTR InstName U2
TEXT -432 40 Left 0 ;.op
TEXT -440 -160 Left 0 !.AC DEC 100 1 100MEG
TEXT -432 -40 Left 0 ;.nodeset V(out)=2 V(in-)=1 V(in+)=1
TEXT -432 -8 Left 0 ;.nodeset V(out1)=0 V(in1-)=0 V(in1+)=0
TEXT -432 -88 Left 0 ;.OPTIONS gmin=1e-10 noopiter=1


Symbol file LMC6484AA.asy

Version 4
SymbolType CELL
LINE Normal -32 32 32 64
LINE Normal -32 96 32 64
LINE Normal -32 32 -32 96
LINE Normal -28 48 -20 48
LINE Normal -28 80 -20 80
LINE Normal -24 84 -24 76
LINE Normal 0 32 0 48
LINE Normal 0 96 0 80
LINE Normal 4 44 12 44
LINE Normal 8 40 8 48
LINE Normal 4 84 12 84
WINDOW 0 16 32 Left 0
WINDOW 3 16 96 Left 0
SYMATTR Value LMC6484A/NS
SYMATTR Prefix X
SYMATTR SpiceModel National.lib
SYMATTR Value2 LMC6484A/NS
SYMATTR Description CMOS Operational Amplifier
PIN -32 80 NONE 0
PINATTR PinName In+
PINATTR SpiceOrder 1
PIN -32 48 NONE 0
PINATTR PinName In-
PINATTR SpiceOrder 2
PIN 0 32 NONE 0
PINATTR PinName V+
PINATTR SpiceOrder 3
PIN 0 96 NONE 0
PINATTR PinName V-
PINATTR SpiceOrder 4
PIN 32 64 NONE 0
PINATTR PinName OUT
PINATTR SpiceOrder 5




File national.lib

* National Semiconductor, Inc.

*/////////////////////////////////////////////////////////////////////

* Legal Notice: This material is intended for free software support.
* The file may be copied, and distributed; however, reselling the
* material is illegal

*////////////////////////////////////////////////////////////////////

* For ordering or technical information on these models, contact:
* National Semiconductor's Customer Response Center
* 7:00 A.M.--7:00 P.M. U.S. Central Time
* (800) 272-9959
* For Applications support, contact the Internet address:
* amps-apps@g...

*//////////////////////////////////////////////////////////
*LMC6484A CMOS Quad OP-AMP MACRO-MODEL
*//////////////////////////////////////////////////////////
*
* connections: non-inverting input
* | inverting input
* | | positive power supply
* | | | negative power supply
* | | | | output
* | | | | |
* | | | | |
.SUBCKT LMC6484A/NS 1 2 99 50 40
* CAUTION: SET .OPTIONS GMIN=1E-16 TO CORRECTLY MODEL INPUT BIAS
CURRENT.
*
*Features:
*Operates from single or dual supplies
*Rail-to-rail input and output swing
*Ultra low input current = 10fA
*Slew rate = 1.2V/uS
*
*NOTE: Model is for single device only and simulated
* supply current is 1/4 of total device current.
* Noise is not modeled.
* Asymmetrical gain is not modeled.
*
**INPUT STAGE****
*
I1 99 4 17U
M1 5 2 4 99 MOSFET
R3 5 50 5.651K
M2 6 7 4 99 MOSFET
R4 6 50 5.651K
*Fp2=5.9 MHz
C4 5 6 2.3868P
G0 98 9 6 5 4.4165E-2
R0 98 9 1K
DP1 1 99 DA
DP2 50 1 DB
DP3 2 99 DB
DP4 50 2 DA
*For accurate Ib , set GMIN<=1E-16 on .OPTIONS line.
*
*COMMON MODE EFFECT*
*
I2 99 50 420.5U
*^Quiescent current
EOS 7 1 POLY(1) 16 49 .75E-3 1
*Offset voltage..........^
R8 99 49 40K
R9 49 50 40K
*
POLE STAGE
*
*Fp=13.3 MHz
G3 98 15 9 49 1E-3
R12 98 15 1K
C5 98 15 11.967P
*
**POLE/ZERO STAGE***
*
*Fp=600 KHz, Fz= 1.4MHz
G5 98 18 15 49 1E-3
R14 98 18 1K
R15 98 19 750
C6 19 18 151.58P
*
****COMMON-MODE ZERO STAGE****
*
*Fpcm=20 KHz
G4 98 16 POLY(2) 1 49 2 49 0 2.812E-8 2.812E-8
L2 98 17 7.958M
R13 17 16 1K
*
****SECOND STAGE****
*
EH 99 98 99 49 1
G1 98 29 18 49 5.6667E-6
R5 98 29 100.37MEG
V2 99 8 1.56
D1 29 8 DX
D2 10 29 DX
V3 10 50 1.56
*
****OUTPUT STAGE****
*
F6 99 50 VA7 1
*^Dynamic supply current
F5 99 35 VA8 1
D3 36 35 DX
VA7 99 36 0
D4 35 99 DX
E1 99 37 99 49 1
VA8 37 38 0
G6 38 40 49 29 16.667E-3
R16 38 40 2.3886K
V4 30 40 .77
D5 30 99 DX
V5 40 31 .77
D6 50 31 DX
*Fp1=2.343 Hz
C3 29 39 17P
R6 39 40 1K
*
MODELS USED****
*
.MODEL DA D(IS=2E-14)
.MODEL DB D(IS=1E-14)
.MODEL DX D(IS=1E-14)
.MODEL MOSFET PMOS(VTO=0 KP=1.842E-3)
.ENDS
*$

Thank you Helmut!
It works now, although when I used your model, I got the "Too few
nodes: current" message. I did not use your example file because of
the different file structure (paths) on my computer. All worked well
though with the model I downloaded from the National site yesterday.
Now I guess I know where my error was - I tried to use a ready symbol
from the library whereas I should have created my own for each 'new'
part I want to use.
Best regards,
Eugene