|
Looking for ideal fully differential amplifier spice model for XSPICE simulations. The one I have based on the XSPICE "gain" code model doesn't have any CMRR or care if outputs are swapped. Anything based on dependent sources would be good.
?
* XSPICE Fully Differential OpAmp
.subckt opamp inp inn outp outn in_offset=0 gain=300e3 out_offset=0
aint %vd(inp inn) %vd(outp outn) amp
.model amp gain (in_offset='in_offset' gain='gain' out_offset='out_offset')
.ends opamp
?
The SE output OpAmp using the same structure works fine...
?
|
On Sat, Dec 21, 2024 at 11:09 PM, Tom wrote:
Looking for ideal fully differential amplifier spice model for XSPICE simulations.
I am a little confused about the request.? Does that mean you want a model that will be used in XSPICE?? Or one for LTspice that behaves similarly to a model you already have for XSPICE?
?
If it is for LTspice, can it be for LTspice only (using LTspice-unique constructs)?
?
Andy
?
|
The generic Spice model would be usable in LTspice or Spice programs that support XSPICE. I found 2 on this forum from 2011 using various search terms.
?
There are many choices for an generic OpAmp with SE output but it seems few for DE output.
|
Tom,
?
Maybe you did not understand my question.
?
Are you looking for a model to run in LTspice, or are you looking for a model to run in XSPICE (or other SPICE programs)?
?
The ideal op-amp models that come with LTspice have single-ended outputs so they are not what you are looking for -- but my point is that it is an LTspice-unique model making it something that would not run in XSPICE or other SPICE programs.
?
So -- here it is again -- are you looking for a model that runs in LTspice, or are you looking for a model that runs in XSPICE?? If someone made a modification of the LTspice ideal op-amp model with differential outputs, would that satisfy your needs, knowing that it does not play with XSPICE?
?
Andy
?
|
Yes, because it's quite easy, and probably
cheaper, to use 2 or 3 sections of a quad opamp to make a good
balanced-in/balanced-out circuit.
On 2024-12-22 13:31, Tom via groups.io
wrote:
The generic Spice model would be usable in LTspice or Spice
programs that support XSPICE. I found 2 on this forum from 2011
using various search terms.
?
There are many choices for an generic OpAmp with SE output
but it seems few for DE output.
--
OOO - Own Opinions Only
Best Wishes
John Woodgate
Keep trying
|
A model that would work for both LTspice and any Spice 3 simulator. The model will also be used in mixed-mode simulations with XSPICE models.?
|
On Sun, Dec 22, 2024 at 08:46 AM, John Woodgate wrote:
Yes, because it's quite easy, and probably cheaper, to use 2 or 3 sections of a quad opamp to make a good balanced-in/balanced-out circuit.
XSPICE models are minimalistic and designed for speed. Complex models would slow simulations to a crawl. In this case the "XSPICE way" for making a fully differential OpAmp creates a model with limitations and the odd "feature" it doesn't care if inputs or outputs are swapped.
|
Here is the thread I found on fully diff OpAmps
?
?
|
What I mean is that there are few real-life
BIBO opamps,from which SPICE models with real-life features,
such as offset and PSRR could be produced.
On 2024-12-22 15:03, Tom via groups.io
wrote:
On Sun, Dec 22, 2024 at 08:46 AM, John Woodgate wrote:
Yes, because it's quite easy, and probably cheaper,
to use 2 or 3 sections of a quad opamp to make a good
balanced-in/balanced-out circuit.
XSPICE models are minimalistic and designed for speed.
Complex models would slow simulations to a crawl. In this case
the "XSPICE way" for making a fully differential OpAmp creates a
model with limitations and the odd "feature" it doesn't care if
inputs or outputs are swapped.
--
OOO - Own Opinions Only
Best Wishes
John Woodgate
Keep trying
|
On Sun, Dec 22, 2024 at 10:17 AM, John Woodgate wrote:
What I mean is that there are few real-life BIBO opamps,from which SPICE models with real-life features, such as offset and PSRR could be produced.
The BIBO models from TI are incredibly complex. They model? lot of parameters.
?
****
* AC PARAMETERS
**
* CLOSED-LOOP OUTPUT IMPEDANCE VS. FREQUENCY (Zout vs. Freq.)
* CLOSED-LOOP GAIN AND PHASE VS. FREQUENCY ?WITH RL, CL EFFECTS (Acl vs. Freq.)
* COMMON-MODE REJECTION RATIO VS. FREQUENCY (CMRR vs. Freq.)
* POWER SUPPLY REJECTION RATIO VS. FREQUENCY (PSRR vs. Freq.)
* INPUT VOLTAGE NOISE DENSITY VS. FREQUENCY (en vs. Freq.)
**
* DC PARAMETERS
**
* INPUT COMMON-MODE VOLTAGE RANGE (Vcm)
* GAIN ERROR (Eg)
* INPUT BIAS CURRENT VS. INPUT COMMON-MODE VOLTAGE (Ib vs. Vcm)
* INPUT OFFSET VOLTAGE VS. TEMPERATURE (Vos vs. Temp)
* OUTPUT VOLTAGE SWING vs. OUTPUT CURRENT (Vout vs. Iout)
* SHORT-CIRCUIT OUTPUT CURRENT (Isc)
* QUIESCENT CURRENT (Iq)
**
* TRANSIENT PARAMETERS
**
* SLEW RATE (SR)
* SETTLING TIME VS. CAPACITIVE LOAD (ts)
* OVERLOAD RECOVERY TIME (tor)
****
|
But you're not looking for a model of a real-life amp, right?
?
I think you said you wanted an ideal model.? That probably means it is lightweight and should simulate fast.
?
Andy
?
|
Well, it's very difficult to have
'comprehensive' without 'complex', unless you are prepared to
write your own models, or add real-life parameters to existing
simpler models.
On 2024-12-22 15:29, Tom via groups.io
wrote:
On Sun, Dec 22, 2024 at 10:17 AM, John Woodgate wrote:
What I mean is that there are few real-life BIBO
opamps,from which SPICE models with real-life features, such
as offset and PSRR could be produced.
The BIBO models from TI are incredibly complex. They model?
lot of parameters.
?
****
* AC PARAMETERS
**
* CLOSED-LOOP OUTPUT IMPEDANCE VS. FREQUENCY (Zout vs. Freq.)
* CLOSED-LOOP GAIN AND PHASE VS. FREQUENCY ?WITH RL, CL EFFECTS
(Acl vs. Freq.)
* COMMON-MODE REJECTION RATIO VS. FREQUENCY (CMRR vs. Freq.)
* POWER SUPPLY REJECTION RATIO VS. FREQUENCY (PSRR vs. Freq.)
* INPUT VOLTAGE NOISE DENSITY VS. FREQUENCY (en vs. Freq.)
**
* DC PARAMETERS
**
* INPUT COMMON-MODE VOLTAGE RANGE (Vcm)
* GAIN ERROR (Eg)
* INPUT BIAS CURRENT VS. INPUT COMMON-MODE VOLTAGE (Ib vs. Vcm)
* INPUT OFFSET VOLTAGE VS. TEMPERATURE (Vos vs. Temp)
* OUTPUT VOLTAGE SWING vs. OUTPUT CURRENT (Vout vs. Iout)
* SHORT-CIRCUIT OUTPUT CURRENT (Isc)
* QUIESCENT CURRENT (Iq)
**
* TRANSIENT PARAMETERS
**
* SLEW RATE (SR)
* SETTLING TIME VS. CAPACITIVE LOAD (ts)
* OVERLOAD RECOVERY TIME (tor)
****
--
OOO - Own Opinions Only
Best Wishes
John Woodgate
Keep trying
|
Correct. Something simple that won't have any convergence issues.
|
This seems to work. G=100MEG seems a bit much.
?
* Ideal Fully Differential OpAmp
* /g/LTspice/topic/50198770#msg46663
*
.subckt D_OpAmp inp inn outp outn vcm
R1 outp n01 1
R2 n01 outn 1
G1 n01 outp inp inn 100MEG
G2 outn n01 inp inn 100MEG
G3 0 n01 vcm n01 100MEG
.ends D_OpAmp
|
To make an ?IDEAL fully differential amplifier spice model...
Simply use a e or e2 Component with whatever gain you want ( In V/V) as a parameter.
(Right click on it and give value V for gain of 100 )
|
On Sun, Dec 22, 2024 at 08:58 AM, <jad700@...> wrote:
To make an ?IDEAL fully differential amplifier spice model...
Simply use a e or e2 Component with whatever gain you want ( In V/V) as a parameter.
(Right click on it and give value 100 for gain of 100 )
|
On 22/12/2024 17:58, jad700 via
groups.io wrote:
To make an ?IDEAL fully
differential amplifier spice model...
Simply use a e or e2 Component
with whatever gain you want ( In V/V) as a parameter.
(Right click on it and give
value V for gain of 100 )
Real DIDO amps have a common mode voltage input.
--
Regards,
Tony
|
On Sun, Dec 22, 2024 at 11:20 AM, Tom wrote:
...
.subckt D_OpAmp inp inn outp outn vcm
R1 outp n01 1
R2 n01 outn 1
G1 n01 outp inp inn 100MEG
G2 outn n01 inp inn 100MEG
G3 0 n01 vcm n01 100MEG
.ends D_OpAmp
Hmm.? I don't see anything to control the bandwidth.? So it is theoretically flat with 160 dB gain from DC to light.
?
It might work.? Or it might not.? Any good op-amp, either a model or real, should have a dominant pole giving it a controlled roll-off as you go up in frequency.
?
And of course the model has no supply voltages, so its inputs and outputs are compliant to +/- infinity - which could be how you want an ideal model to be.
?
Andy
?
?
|
It's primary use is for XSPICE mixed-mode simulations. For XSPICE the key is simplicity so simulation times are reasonable. I needed something quick to replace the original code model used in a Sigma-Delta converter example. I look forward to better models with user configured parameters.?
|
Screen shot of Delta-Sigma Converter uploaded
|
John Woodgate
Tony Casey