Keyboard Shortcuts
Лайки
Пошук
Looking for ideal fully differential amplifier spice model
12/22/24
#156949
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:
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
|
12/22/24
#156951
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:
-- OOO - Own Opinions Only Best Wishes John Woodgate Keep trying |
12/22/24
#156956
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. |
12/22/24
#156957
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. |
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:
-- OOO - Own Opinions Only Best Wishes John Woodgate Keep trying |
12/22/24
#156960
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) ****************************************************** |
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:
-- OOO - Own Opinions Only Best Wishes John Woodgate Keep trying |
12/22/24
#156965
This seems to work. G=100MEG seems a bit much.
* Ideal Fully Differential OpAmp * https://groups.io/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 |
On 22/12/2024 17:58, jad700 via
groups.io wrote:
Real DIDO amps have a common mode voltage input. -- Regards,
Tony |
On Sun, Dec 22, 2024 at 11:20 AM, Tom wrote:
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
|
12/23/24
#156994
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. |
Повідомлення
Більше