spice model for ts972 opamp?

[Joe]

Does anyone know where I may find a spice model or subckt of this opamp? It
is mfg by STmicroelectronics. I visited their site, and could not find it.
FYI , they do have models of their mosfets . I also tried to find a cross
reference with another company's part number, but no luck there either.

Any help greatly appreciated. I am using LTSPICE.

TIA,
Joe

 

[Kevin Aylward]

Does anyone know where I may find a spice model or subckt of this
opamp? It is mfg by STmicroelectronics. I visited their site, and
could not find it. FYI , they do have models of their mosfets . I
also tried to find a cross reference with another company's part
number, but no luck there either.

Any help greatly appreciated. I am using LTSPICE.

Since you are using the model, you must know what its basic
characteristics are. In this case, chose a similar op-model.

Kevin Aylward
[email protected]
http://www.anasoft.co.uk
SuperSpice, a very affordable Mixed-Mode
Windows Simulator with Schematic Capture,
Waveform Display, FFT's and Filter Design.

"quotes with no meaning, are meaningless" - Kevin Aylward.

 

[Jim Thompson]

Does anyone know where I may find a spice model or subckt of this opamp? It
is mfg by STmicroelectronics. I visited their site, and could not find it.
FYI , they do have models of their mosfets . I also tried to find a cross
reference with another company's part number, but no luck there either.

Any help greatly appreciated. I am using LTSPICE.

TIA,
Joe

Download the configurable OpAmp subcircuit from my website and then
fill in the blanks for gain, gain-bandwidth and phase margin.

...Jim Thompson

 

[Mike Engelhardt]

Joe,

Download the configurable OpAmp subcircuit from my website
and then fill in the blanks for gain, gain-bandwidth and
phase margin.

In LTspice, there's a symbol, UniversalOpamp. You can
specify gain(Avol), gain-bandwidth, phase margin, slew
rate limit, current limit, how close the output goes to
the rails, and full noise parameters. There's two
different underlying implementations to for the phase
margin to choose from. You're probably better of with
that model for any generic opamp then even the elaborate
vender-supplied opamp macro models.

--Mike

 

[Tim Stinchcombe]

Does anyone know where I may find a spice model or subckt of this opamp? It
is mfg by STmicroelectronics. I visited their site, and could not find it.
FYI , they do have models of their mosfets . I also tried to find a cross
reference with another company's part number, but no luck there either.

Any help greatly appreciated. I am using LTSPICE.

It appears to be here:

http://www.st.com/stonline/products/support/macromdl/stdlnr/ts97x.txt

Oftentimes when searching manufacturers sites you have to be very
persistent: in this case looking under 'support'!

Tim

 

[Joe]

Since you are using the model, you must know what its basic
characteristics are. In this case, chose a similar op-model.

Kevin Aylward
[email protected]
http://www.anasoft.co.uk
SuperSpice, a very affordable Mixed-Mode
Windows Simulator with Schematic Capture,
Waveform Display, FFT's and Filter Design.

"quotes with no meaning, are meaningless" - Kevin Aylward.

Hi Kevin,

Thank you for your reply. I am not sure what you mean by basic
characteristics. I have the data sheet and I see that it is a rail to rail,
low noise opamp, with supply voltages from 2.7V to 10V. It has a GBW of
12MHZ and slew rate of 4V/us. I think I know how to read the data sheet, but
creating a model from it is beyond me right now. I also did not really want
to go looking at every other opamp data sheet to first see if there was one
that was similar, and second, to see if there was an existing model for
LTSPICE.

Joe

 

[Joe]

Download the configurable OpAmp subcircuit from my website and then
fill in the blanks for gain, gain-bandwidth and phase margin.

...Jim Thompson

Hi Jim,

Thank you for the link to your model.
I downloaded your configurable opamp subcircuit and read the text directions
that came with it. This looks like it can be a really easy way to create new
opamp models as I discover them.

I cannot find a parameter called dc gain on the data sheet, and also could
not find anything called open loop output resistance. Do you think it is OK
if I use the defaults for those? I found all the other parameters on the
data sheet.

Also, this subckt does not seem to be in the same format as a LTSPICE
subckt.
Your first line is: .SUBCKT OP-AMP-CONFIG INP INN OUT
The models and subckts I have seen in LTSPICE have something like this:
..subckt op-amp-config 1 2 3 4 5

where the numbers designate the noninverting input, inverting input,
positive power supply, negative power supply, and output. They can be any
numbers, from what I have seen, as long as there's 5 of them. Can I put
these numbers in without disrupting your model?

Thanks,
Joe

 

[Joe]

Joe,


In LTspice, there's a symbol, UniversalOpamp. You can
specify gain(Avol), gain-bandwidth, phase margin, slew
rate limit, current limit, how close the output goes to
the rails, and full noise parameters. There's two
different underlying implementations to for the phase
margin to choose from. You're probably better of with
that model for any generic opamp then even the elaborate
vender-supplied opamp macro models.

--Mike

Hi Mike,
Thank you for the reply. This is a great feature that I did not know about
in LTSPICE.

I have been looking it over . It actually contains 5 subcircuits. I was not
sure which one to use, or are they all needed?
Each one looks like it describes an opamp. Also, I am not sure where to put
the parameters you specified above. Do they go in the .param statements? I
looked in the help file and I could not seem to find anything on using the
universal opamp model. Just looking at the first subckt (.subckt level 1), I
know that GBW is GBP on the data sheet, and PM is phase margin, Slew would
be slew rate, but not sure about the following:
Rout,Avol,ilimit,rail, vos,en,enk,in,ink. and what these are called on the
data sheet.

Also, once I sort this out and have the subckt, can I use the LT1013 as the
..asy? I usually use that for new opamp models I find.

Thanks,
Joe

 

[Jim Thompson]

Download the configurable OpAmp subcircuit from my website and then
fill in the blanks for gain, gain-bandwidth and phase margin.

...Jim Thompson

[snip]

Hi Jim,

Thank you for the link to your model.
I downloaded your configurable opamp subcircuit and read the text directions
that came with it. This looks like it can be a really easy way to create new
opamp models as I discover them.

I cannot find a parameter called dc gain on the data sheet, and also could
not find anything called open loop output resistance. Do you think it is OK
if I use the defaults for those? I found all the other parameters on the
data sheet.

Also, this subckt does not seem to be in the same format as a LTSPICE
subckt.
Your first line is: .SUBCKT OP-AMP-CONFIG INP INN OUT
The models and subckts I have seen in LTSPICE have something like this:
.subckt op-amp-config 1 2 3 4 5

where the numbers designate the noninverting input, inverting input,
positive power supply, negative power supply, and output. They can be any
numbers, from what I have seen, as long as there's 5 of them. Can I put
these numbers in without disrupting your model?

Thanks,
Joe

I'm sure that LTSpice supports node NAMES, and my model only uses
three nodes... you can number them as 1 2 3 if you like, but you will
have to appropriately edit the subcircuit so that the header
declaration match the node names below in the netlist (below header
and before ".ENDS")

...Jim Thompson

 

[Joe]

It appears to be here:

http://www.st.com/stonline/products/support/macromdl/stdlnr/ts97x.txt

Oftentimes when searching manufacturers sites you have to be very
persistent: in this case looking under 'support'!

Tim

--
__________________________________________________________
Tim Stinchcombe

Cheltenham, Glos, UK

Hi Tim,

I got it, now I have 3 subcircuits to play with and see which one is more
accurate. I noticed that they put the inputs in a different order than is
standard in LTSPICE, so I will have to see if I can change them to be in the
right order without screwing up the subcircuit.

Thank you for the link. I would have never thought to look in 'support'.

Joe

 

[Mike Engelhardt]

Joe,

In LTspice, there's a symbol, UniversalOpamp. You can
specify gain(Avol), gain-bandwidth, phase margin, slew
rate limit, current limit, how close the output goes to
the rails, and full noise parameters. There's two
different underlying implementations to for the phase
margin to choose from. You're probably better of with
that model for any generic opamp then even the elaborate
vender-supplied opamp macro models.

I have been looking it over . It actually contains
5 subcircuits...I looked in the help file and I could
not seem to find anything on using the universal opamp
model.

See the file ./examples/Educational/UniversalOpamp.asc. You
choose the level you wish to use for simulation. Higher levels
simulate more aspects of the opamp at the expense of internal
complexity.

I was not sure which one to use, or are they all needed? Each
one looks like it describes an opamp.

When you include an instance of the UniversalOpamp symbol,
all of them get defined, but only the level you wish is used.

Also, I am not sure where to put the parameters you specified
above. Do they go in the .param statements?

Right click on a UniversalOpamp after you put one on a schematic.
Set the simulation level and edit the parameters there.

Rout,Avol,ilimit,rail, vos,en, enk,in,ink. and what these
are called on the data sheet.

Rout : internal use only
Avol : DC gain
ilimit: output current limit
rail : How close the output gets to the power rails
vos : offset voltage
en : equiv. input voltage noise density
enk : equiv. input voltage noise density corner freq.
in : equiv. input current noise density
ink : equiv. input current noise density corner freq.

Also, once I sort this out and have the subckt, can I
use the LT1013 as the .asy? I usually use that for new
opamp models I find.

The LT1013 symbol is wired to a specific model, not
the universal opamp. The universal opamp uses special
LTspice internal devices like a transconductance with
a hyperbolic transfer function to model slew rate and
the onset of slew rate limited distortion into the
dominate pole's capacitance.

--Mike

 

[Joe]

Joe,



See the file ./examples/Educational/UniversalOpamp.asc. You
choose the level you wish to use for simulation. Higher levels
simulate more aspects of the opamp at the expense of internal
complexity.


When you include an instance of the UniversalOpamp symbol,
all of them get defined, but only the level you wish is used.


Right click on a UniversalOpamp after you put one on a schematic.
Set the simulation level and edit the parameters there.


Rout : internal use only
Avol : DC gain
ilimit: output current limit
rail : How close the output gets to the power rails
vos : offset voltage
en : equiv. input voltage noise density
enk : equiv. input voltage noise density corner freq.
in : equiv. input current noise density
ink : equiv. input current noise density corner freq.


The LT1013 symbol is wired to a specific model, not
the universal opamp. The universal opamp uses special
LTspice internal devices like a transconductance with
a hyperbolic transfer function to model slew rate and
the onset of slew rate limited distortion into the
dominate pole's capacitance.

--Mike

Thank you Mike, I will give it a try.

Joe