Whats missing in this diode model ?

[MathWizard]

I'm modelling a used, linear PSU I have, and in a bias chain, LTS says it would have ~176.6uA of current. The closest I can calculate is 180.3uA, which is still only up by 2%. The bias chain alone, is just 2x 9V1zen, 2x 1N4148, and 160k, all in series between 48V total.

I'm using the zener voltage that LTspice gets, and then a starting guess for Vd of the 1N4148, and solving for the current from all those known voltages and R. Then using that current in the Shockley diode eqn (w/ the param's from LTS, Is=2.52nA , n=1.752, Rs=0.568 ), to get a new Vd. Then iterating that sequence from Vd to Id, until the difference between the new and last Vd, is below ~10E-15, and then the spreadsheet considers it zero.

I'm was using a 9V1 zener BZX84C9V1LY, it has a low Is, and in circuit LTS has Vz=9.0734329V, and my Vd calc gets to +0.143% of the LTS value, but the current is off by +2%

With KDZ9_1B or PTZ9_1B, w/ 1000x and 100,000x the Is of the above, I still only get within 0.3% for Vd and 2-3% for Id


So what other little fudge factor, or parameter, like Early voltage for BJT's , and the (1+VCE/VA) term for BJT's, can I use for a regular diode ?



For DC biasing, I've just worked backwards, calculating "everything" from the output of a 30V PSU, only ignoring a couple of things that I could have added in. And also using the zener voltages from LTS, and the effective beta of 2 driver BJT's.

And going around the voltage control loop, all my calculations are within +/-0.9% of the real model with a 2SC1085, TIP31C, and 2N3055, and LM301A, for ALL currents and voltages, even for nA levels of current.

But the thing that's off the most by about 6% or 6uA (in that circuit), is this bias chain with these zener's and diodes. If I can get all those V's and I's for the BJT's and op-amp within 0.9% or better (most of them are 99.9% or better) using similar methods and equations with the basic BJT model, I'd figure this bias chain would match even better than those.

[mawyatt]

Are you using same Temperature as Spice simulations?

The models may use 25C (298K) or 27C (300K) as normalized "Room Temp" ambient.

Best

[MathWizard]

The Vt I was using is 0.025852V, so thats right around there. And Id=(Vcc-Vee-2*Vz-2*Vd)/R, and for the Vd, the Rs didn't matter, so I'm using Vd=nVt*LN(Id/Is).

If I use Vd=nVt*LN(Id/Is+1) , then Id is down -0.3%, and Vd is -2.5% off, and that Vt for be for 300Kelvin. OK I'll play the temperature, see if that fixes it. But that's the same Vt I use for BJTs.

No w/ Vd=nVt*LN(Id/Is+1), that barely changed anything I had a different zener a moment ago. And changing T by a few degrees in Vt=kT/q, only changes the Vd a little, and barely changes Id

[MathWizard]

All the articles and examples I've found, are using the same diode eqn's as I am, for 26.85C=300K, and the 1N4148 is just the default one included in LTS.

Id=Is*[ exp( (Vd-Rs*Id)/(nVt) ) - 1]      Vd = nVt*LN[(Id/Is)+1] + Rd*Id

I'm getting back into the Ebers-Moll eqns and the modified Gummel-Poon model for BJT's. I got carried away with how accurate my PSU calulations were, but it was only for 30V, 3mA. The same eqn's go way off as the current goes up.

And so far I haven't found any more detailed eqn for a diode, besides semi-conductor physics books, so what it LTS doing? Or what method does it use to calculate it ?

I know I don't have to get the same answer, and it's just a simulator.

[mawyatt]

The voltage across the diode junction is not the same as the voltage across the diode terminals, the terminals include the diode series resistor effects, so the actual junction is slightly lower than what is across the diode terminals.

BTW the solution to a simple diode with a junction with a series resistance is transcendental!!

Best,

[TimFox]

The voltage across the diode junction is not the same as the voltage across the diode terminals, the terminals include the diode series resistor effects, so the actual junction is slightly lower than what is across the diode terminals.

BTW the solution to a simple diode with a junction with a series resistance is transcendental!!

Best,

If you need to calculate the I-V curve of a junction and series resistance, you can straightforwardly calculate the total voltage as a function of current, by calculating the voltage across each element for the same current and summing them.
However, if you try to calculate the current as a function of voltage, you will have transcendental problems.