Maker Pro
Maker Pro

Problems with SPICE models from vendors

R

Robert Baer

Jan 1, 1970
0
The LM324 model from TI works fine,but the one from National
Semiconductor is junk.
I tried numerous Analog Devices models for various rail-to-rail
opamps, and found that almost all i tried gave me the same kind of
cryptic square root error.
Those tried: AD8605, AD531, AD541, AD8552, and the AD8571; the only
one tried that did work was for the AD8614.
Now i would dearly like to have a set of models that were known to
work (and more or less correctly), but i need to get a working AD8605 model.
The sets i have came from the manufacturer created in the latter of
1992, and thus are not quite up-to-date.
However, the model for the AD8605 was downloaded via the web just
yesterday - implying the problem is not fixed.

Can anyone help?
 
H

Helmut Sennewald

Jan 1, 1970
0
Robert Baer said:
The LM324 model from TI works fine,but the one from National
Semiconductor is junk.
I tried numerous Analog Devices models for various rail-to-rail opamps,
and found that almost all i tried gave me the same kind of cryptic square
root error.
Those tried: AD8605, AD531, AD541, AD8552, and the AD8571; the only one
tried that did work was for the AD8614.
Now i would dearly like to have a set of models that were known to work
(and more or less correctly), but i need to get a working AD8605 model.
The sets i have came from the manufacturer created in the latter of
1992, and thus are not quite up-to-date.
However, the model for the AD8605 was downloaded via the web just
yesterday - implying the problem is not fixed.

Can anyone help?

Hello Robert,
I don't believe that you really can judge the quality of these
models as a beginner with SPICE simulations.
I agree with you that most models have difficulties with convergence.
Many of them are really over complicated and sometimes generated
by stupid programs or "roboters" and not by engineers.

I assume that the listed models will work with some tweaking
of the convergence parameters.

What simulator do you use?
If it's LTspice then send me your files and I will make
you a working example with your AD8605.
I always want to see the schematic, because I know that
people sometimes have errors in their circuit.
One important thing is to have a DC path to ground(0).


Best Regards,
Helmut
Moderator of the LTspice user group
 
J

Jim Thompson

Jan 1, 1970
0
The LM324 model from TI works fine,but the one from National
Semiconductor is junk.
I tried numerous Analog Devices models for various rail-to-rail
opamps, and found that almost all i tried gave me the same kind of
cryptic square root error.
Those tried: AD8605, AD531, AD541, AD8552, and the AD8571; the only
one tried that did work was for the AD8614.
Now i would dearly like to have a set of models that were known to
work (and more or less correctly), but i need to get a working AD8605 model.
The sets i have came from the manufacturer created in the latter of
1992, and thus are not quite up-to-date.
However, the model for the AD8605 was downloaded via the web just
yesterday - implying the problem is not fixed.

Can anyone help?

Problem noted, and forwarded to the appropriate device-modeling
manager at Analog Devices.

I, personally, have experienced some problems with ADI models.
Reported same, and was told, "They work just fine here."

So don't hold your breath.

BTW, Sennewald is wrong when he says, "...generated by stupid programs
or "roboters" and not by engineers."

They ARE generated by engineers, or should I say it as "engineers"
?:)

...Jim Thompson
 
H

Helmut Sennewald

Jan 1, 1970
0
----- Original Message -----
From: "Jim Thompson" <[email protected]>
Newsgroups: sci.electronics.cad
Sent: Friday, March 25, 2005 3:37 PM
Subject: Re: Problems with SPICE models from vendors

Problem noted, and forwarded to the appropriate device-modeling
manager at Analog Devices.

Hello Jim,
this wasn't necessary. This AD8605 model runs without any
convergence problem in LTspice. So the model doesn't have any error.
Yuu should withdraw your email to AD and apologize to the manager
you have contacted for any inconvenience. :)

Best Regards,
Helmut
 
J

Jim Thompson

Jan 1, 1970
0
----- Original Message -----
From: "Jim Thompson" <[email protected]>
Newsgroups: sci.electronics.cad
Sent: Friday, March 25, 2005 3:37 PM
Subject: Re: Problems with SPICE models from vendors



Hello Jim,
this wasn't necessary. This AD8605 model runs without any
convergence problem in LTspice. So the model doesn't have any error.
Yuu should withdraw your email to AD and apologize to the manager
you have contacted for any inconvenience. :)

Best Regards,
Helmut

I simply passed on the posting to the ADI manager.

As previously noted, I, personally, have experienced issues with ADI
models.

...Jim Thompson
 
J

Jim Thompson

Jan 1, 1970
0
I simply passed on the posting to the ADI manager.

As previously noted, I, personally, have experienced issues with ADI
models.

...Jim Thompson

But the AD8605 seems to NOT be one of them. Works AOK on PSpice.

Results conveyed to JA at ADI.

...Jim Thompson
 
hello folks, just saw your message about my Spice models. I did the
AD8605 model and would like to know what it is that you think isn't
working. I would prefer to see the test circuit you're using and
understand what you're trying to do. And if it really doesn't work,
then I owe you a pizza of your choice.
 
H

Helmut Sennewald

Jan 1, 1970
0
hello folks, just saw your message about my Spice models. I did the
AD8605 model and would like to know what it is that you think isn't
working. I would prefer to see the test circuit you're using and
understand what you're trying to do. And if it really doesn't work,
then I owe you a pizza of your choice.

Good morning Sir,
I posted 2h40m ago that this model has no problem.
Have you overlooked that or do you do you see postings only
after many hours? Please use a better news reader.
May news reader is uptodate within minutes.

Best Regards,
Helmut



My posting from 2h40m ago:
Problem noted, and forwarded to the appropriate device-modeling
manager at Analog Devices.

Hello Jim,
this wasn't necessary. This AD8605 model runs without any
convergence problem in LTspice. So the model doesn't have any error.
Yuu should withdraw your email to AD and apologize to the manager
you have contacted for any inconvenience. :)

Best Regards,
Helmut
 
J

Jim Thompson

Jan 1, 1970
0
Good morning Sir,
I posted 2h40m ago that this model has no problem.
Have you overlooked that or do you do you see postings only
after many hours? Please use a better news reader.
May news reader is uptodate within minutes.

Best Regards,
Helmut



My posting from 2h40m ago:


Hello Jim,
this wasn't necessary. This AD8605 model runs without any
convergence problem in LTspice. So the model doesn't have any error.
Yuu should withdraw your email to AD and apologize to the manager
you have contacted for any inconvenience. :)

Best Regards,
Helmut

I have also checked it independently myself, on PSpice v10.3.

NO PROBLEM!

...Jim Thompson
 
R

Robert Baer

Jan 1, 1970
0
Helmut said:
Hello Robert,
I don't believe that you really can judge the quality of these
models as a beginner with SPICE simulations.
I agree with you that most models have difficulties with convergence.
Many of them are really over complicated and sometimes generated
by stupid programs or "roboters" and not by engineers.

I assume that the listed models will work with some tweaking
of the convergence parameters.

What simulator do you use?
If it's LTspice then send me your files and I will make
you a working example with your AD8605.
I always want to see the schematic, because I know that
people sometimes have errors in their circuit.
One important thing is to have a DC path to ground(0).


Best Regards,
Helmut
Moderator of the LTspice user group
Well, in a sense you are correct in labellling be as a beginner; i
rarely use SPICE, but that useage has covered over 30 years.
When one models a simple voltage follower, with the NI input half way
between the poser supplies for the op-amp, one expects it to work, and
not give a cryptic square root error.
Furthermore, replacing the model used to a different one (eg replace
the call from the AD8605 to the AD8614 (and changing *nothing* else) and
have it work begs the question: what is wrong with the AD8605 model?
The same can be said about the models for the LM324; the TI model
works and the NatSemi does not.

And speaking of bad models that DO "work", the AD8614 is rather poor
(from the .OUT file):

.OPTIONS ACCT LIST NODE OPTS NUMDGT=6 RELTOL=0.00001 NOPAGE
.TEMP 27
.LIB ANLG_DEV.LIB ; most rail-to-rail opamps die with error
.DC VBAT 4.499 4.501 0.001
VBAT 01 00 DC 4.5
VSET 10 00 0.209171
VIN 05 00 0.018051
R2 05 07 18.4K
R3 10 08 18.4K
R4 09 07 100K
* NI I OUT
XAMP2 08 07 01 00 09 AD8614/AD
.PRINT DC V(05) V(07) V(08) V(09)
.PLOT DC V(05) V(07) V(08) V(09)
.SAVE

V(5) V(7) V(8) V(9)

1.80510E-02 2.22746E-01 2.21746E-01 1.26487E+00

Look at the poor results: large input currents, large Vos. Almost
useless; certainly not representative of the part.
 
R

Robert Baer

Jan 1, 1970
0
Jim said:
Problem noted, and forwarded to the appropriate device-modeling
manager at Analog Devices.

I, personally, have experienced some problems with ADI models.
Reported same, and was told, "They work just fine here."

So don't hold your breath.

BTW, Sennewald is wrong when he says, "...generated by stupid programs
or "roboters" and not by engineers."

They ARE generated by engineers, or should I say it as "engineers"
?:)

...Jim Thompson
I appreciate that you passed on the comments.
Please see my slightly earlier response, showing problems with the
AD8614 (high input currents and high Vos).
 
R

Robert Baer

Jan 1, 1970
0
Helmut said:
----- Original Message -----
From: "Jim Thompson" <[email protected]>
Newsgroups: sci.electronics.cad
Sent: Friday, March 25, 2005 3:37 PM
Subject: Re: Problems with SPICE models from vendors





Hello Jim,
this wasn't necessary. This AD8605 model runs without any
convergence problem in LTspice. So the model doesn't have any error.
Yuu should withdraw your email to AD and apologize to the manager
you have contacted for any inconvenience. :)

Best Regards,
Helmut
Please tell me why it does not work (and others mentioned) and that
the model for the AD8614 does work.
I am using a DOS version of TopSpice.
And look at an earlier posting where i clearly show that the AD8614
model gives large input currents and a large Vos.
 
R

Robert Baer

Jan 1, 1970
0
hello folks, just saw your message about my Spice models. I did the
AD8605 model and would like to know what it is that you think isn't
working. I would prefer to see the test circuit you're using and
understand what you're trying to do. And if it really doesn't work,
then I owe you a pizza of your choice.








only one


to work
Here is a partial of the .OUT for the AD8614 which "works":
.OPTIONS ACCT LIST NODE OPTS NUMDGT=6 RELTOL=0.00001 NOPAGE
.TEMP 27
.LIB ANLG_DEV.LIB ; most rail-to-rail opamps die with square
root error
.DC VBAT 4.499 4.501 0.001
VBAT 01 00 DC 4.5
VSET 10 00 0.209171
VIN 05 00 0.018051
R2 05 07 18.4K
R3 10 08 18.4K
R4 09 07 100K
* NI I OUT
XAMP2 08 07 01 00 09 AD8614/AD ;AD8605 U2
.PRINT DC V(05) V(07) V(08) V(09)
.PLOT DC V(05) V(07) V(08) V(09)
.SAVE

V(5) V(7) V(8) V(9)

1.80510E-02 2.22746E-01 2.21746E-01 1.26487E+00

Note the large input currents and large Vos.
Will see if i can run my DOS TopSpice when online...
***********
Well, the error message is only on the screen, and it is hard to read.
If i interpreted it correctly, it states "run time error M6201: MATH
-sqrt: DOMAIN error".
I hope this information is of some use.
Meanwhile, maybe i can figure out how to download LTspice (if it is
not gigantic, as i am on POTS).

***********
 
J

Jim Thompson

Jan 1, 1970
0
Well, in a sense you are correct in labellling be as a beginner; i
rarely use SPICE, but that useage has covered over 30 years.
When one models a simple voltage follower, with the NI input half way
between the poser supplies for the op-amp, one expects it to work, and
not give a cryptic square root error.
Furthermore, replacing the model used to a different one (eg replace
the call from the AD8605 to the AD8614 (and changing *nothing* else) and
have it work begs the question: what is wrong with the AD8605 model?
The same can be said about the models for the LM324; the TI model
works and the NatSemi does not.

And speaking of bad models that DO "work", the AD8614 is rather poor
(from the .OUT file):

.OPTIONS ACCT LIST NODE OPTS NUMDGT=6 RELTOL=0.00001 NOPAGE
.TEMP 27
.LIB ANLG_DEV.LIB ; most rail-to-rail opamps die with error
.DC VBAT 4.499 4.501 0.001
VBAT 01 00 DC 4.5
VSET 10 00 0.209171
VIN 05 00 0.018051
R2 05 07 18.4K
R3 10 08 18.4K
R4 09 07 100K
* NI I OUT
XAMP2 08 07 01 00 09 AD8614/AD
.PRINT DC V(05) V(07) V(08) V(09)
.PLOT DC V(05) V(07) V(08) V(09)
.SAVE

V(5) V(7) V(8) V(9)

1.80510E-02 2.22746E-01 2.21746E-01 1.26487E+00

Look at the poor results: large input currents, large Vos. Almost
useless; certainly not representative of the part.

For the rated VCC (+5V and up), I'm getting offset right at the
typical of 1mV.

BUT the IB's are about double the MAX spec.

...Jim Thompson
 
Hmm useless huh? the AD8614 has 1mV of Vos and the model has 1mV, I
just looked at it, so I don't know what you mean by not working. I
think you may be overlooking some things here. Here's the Vos in the
netlist...
EOS 7 1 POLY(2) (73,98) (81,98) 1E-3 1 1
 
J

Jim Thompson

Jan 1, 1970
0
Hmm useless huh? the AD8614 has 1mV of Vos and the model has 1mV, I
just looked at it, so I don't know what you mean by not working. I
think you may be overlooking some things here. Here's the Vos in the
netlist...
EOS 7 1 POLY(2) (73,98) (81,98) 1E-3 1 1
[snip]

I just verified Baer's setup with PSpice. The IB's are running
~700nA, substantially larger than the MAX spec.

I simply visually scanned the data sheet, so I don't know... are we
close enough to negative rail to cause the high IB?

...Jim Thompson
 
H

Helmut Sennewald

Jan 1, 1970
0
Hmm useless huh? the AD8614 has 1mV of Vos and the model has 1mV, I
just looked at it, so I don't know what you mean by not working. I
think you may be overlooking some things here. Here's the Vos in the
netlist...
EOS 7 1 POLY(2) (73,98) (81,98) 1E-3 1 1

Hello zidane,

Robert was especially disappointed about the bias current.
It is modeled with about 700nA.
The datasheet shows max. Ib=400nA.
It's a valid question why Ib is modelled not with the typical values.
The later curves in the datasheet show Ib=300nA.
I am talking about Ib when Vin is near the supply rails.
Maybe you can enlighten us about the bias current.

I agree with your typical Vos of 1mV.

Best Regards,
Helmut
 
H

Helmut Sennewald

Jan 1, 1970
0
Robert Baer said:
Please tell me why it does not work (and others mentioned) and that the
model for the AD8614 does work.
I am using a DOS version of TopSpice.
And look at an earlier posting where i clearly show that the AD8614
model gives large input currents and a large Vos.

Hello Robert,
please tell me who said that the Ad8605 model doesn't work?
Maybe TopSpice has problems with this opamp whereas other SPICE
variants don't have a problem with the AD8605.
The different SPICE versions on the market are far off from the
original SPICE program code.

Best Regards,
Helmut
 
R

Robert Baer

Jan 1, 1970
0
Hmm useless huh? the AD8614 has 1mV of Vos and the model has 1mV, I
just looked at it, so I don't know what you mean by not working. I
think you may be overlooking some things here. Here's the Vos in the
netlist...
EOS 7 1 POLY(2) (73,98) (81,98) 1E-3 1 1







only one


to work
Ok, i am convinced that the AD8614 was a lousy choice - but it was
the only rail-to-rail model that worked at that time.
I have downloaded SwitcherCAD3 and have part of my circuit working
using the AD8605 model.
So it is clear that there is something about those
non-working-for-TopSpice models that goof it up, but is allowed in the
more modern SPICE programs.
That said, the results i get are WRONG - essentially it is saying
that 1+1 is not 2.
I could attach the .ASC file, but it is fairly large (about 4K), and
tell you what the node voltages SC3 gives.
Let me do it the quick way; SC3 sez:
N003 at 0.295mV; R2=18.2K from N003 to N007 at 0.188481V; op amp NI
at N006, I at N007, output at N008, V- at gnd, v+ at 4.5V; feedback
R4=100K from N006 to N007; N006 at 0.188571V; I(R2)=I(R4)=10.3399uA;
N008=0.376666V.

But do the calcs by hand; I(R2) = (0.188481V-0.000295V)/(18.2K) =
0.0103398mA. Drop across 100k then is 1.03398V; add to voltage at N007
for calc(N008)=1.222461V.

Therefore 1+1=2 and Spice is whistling Dixie.
 
Top