PSRR for LDOs using LTSpice

[razor6271]

Hello,
I have been trying to find the PSRR of LT-3094 and LT-3045-1 for my project, but the issue are two folds:
a) My readings do not match those of datasheets, I have been trying to see the effect of voltage and frequency on the PSRR, so I sweep both and then check the PSRR values but they are very erratic.
b) My simulation often stops in between or in the start by saying "Source stepping = 100% , finding iterations..." which never stops until I press "escape" and it gives the simulation but I think that is more of an error and bruteforcing the simulation instead of correct results.

There might be problems with my circuit or my code because I am pretty new to this, so would appreciate any help. Thanks.

 

[D.A.(Tony)Stewart]

zip the files

 

[KlausST]

Hi,

I won´t be surprised if the simulation models are focussed on functional simulation.
This means the models may not be realistic regarding PSRR.
Indeed - I guess - the answer about realistic PSRR simulation can only be given by the model designer.

I would not rely on the simulation results.
For sure PSRR is a function of the feedback loop (which should be modeled properly) .. but also on GND boune, stray capacitance, inductive coupling of several paths on the chip...

Klaus

 

[D.A.(Tony)Stewart]

Process options may need to change from normal to alternate.

 

[crutschow]

I agree that the LTspice model may not accurately show the PSRR.
You likely will have to measure a real circuit to determine that with reasonable accuracy.

 

[danadakk]

Contact Analog Devices engineering and ask if model capable of supporting
your requirements.....

Regards, Dana.

 

[dick_freebird]

Yes, those encrypted macromodels may lack the elements
needed to represent the VCC-VOUT transfer function (as
well as any other paths). SOmebody would have had to
make the effort, unlike transistor-level models which this
would "just fall out of".

Of course being encrypted you don't get to inspect. That's
why.

You might find a schematic made of transistors out there,
some folks make a hobby of that. Not to say, likely. Unless
you happened to pick a popular part that happened to have
such a fan.

Simply, you could set up two DC OP analyses at two
different supply voltages but consistent load and feedback,
and then PSRR is dB20((VOUT2-VOUT1)/(VCC2-VCC1).
You can explain a lack of credible supply driven output
deflection as a lack of macromodeler effort, if challenged.
Doing something about that, though, would slide into reverse
engineering and proprietary SPICE transistor (& passives)
model scrounging.

Might wade into the contrib libs behind LTWiki and see if
any fans left you a bonus...

 

[BigBoss]

PSRR Simulations are NOT done with Transient Analysis.This is fundamental error.
PSRR analysis is done with AC simulation. Simple Out over Simple in in DB.

 

[dick_freebird]

While canonical PSRR may be considered small signal, you would be remiss to assume that incoming supply activity qualifies as such, or will provoke only small response.

Tran is closest to realism while DC and AC analyses rest on assumptions that want careful and constant review, for what they tell and what they hide.

DC analysis for the DC datasheet value. AC analysis for any HF PSRR interest. But Tran to verify that you are getting the whole story as the user in application will see it, and that the two simple analyses are not "dumb and dumber" (like, if the control loop winds up at some supply*load point, you left Kansas some while back).