Compensating the temperature coefficient of a LTZ1000 voltage reference?

[Kleinstein]

This is only a simulation and the models for temperature dependence are often not that good. Usually they don't contain case effects, but more the the theoretical silicone part only.

The OP177 example shows another simulation problem: the real OP177 is not single supply.

[iMo]

Moreover, the opamps models usually do not include the TCs of the drifts. Therefore my note above when somebody tries it out in HW.
Below with LT1013A, 0.13ppm/C (box).

[imisaac]

Thanks imo for the beautiful simulations. Thanks Kleinstein for the deep insights.

I attempted to reproduce your circuit simulation in LTspice, but with a 6.2 V buried zener instead (attached). This was the reference circuit that the following parameter values were derived.

The sensitivity coefficient of the voltage reference out to the resistor R1 (series resistor to the zener) and R3 (collector resistor) were about +0.02 ppm/ppm and -0.005 ppm/ppm respectively.

The observations are:
1. The two sensitivity coefficients were opposite in sign.
2. The zener series resistor had the much stronger effect in the system tempco.
3. The zero tempco operating temperature was about 22.3 ^oC.

If I use a resistor with a tempco of 5 ppm/^oC for both R1 and R3 and operate the system at the "zero tempco" temperature, then the system temco would be 0.1 ppm/^oC, mainly dominated by R1. This represents the lower bound for the topology and component specs used.

The tempco of R1 seems to be very critical.

[Kleinstein]

The sensitivity to R1 changes is the main problem with the TC adjustment. Here it is not only the TC of R1, but also the long term drift of R1 that is a problem.

Where the zero TC point is depends on the details and exact values. So with suitable resistor values one can chose the value.
When an oven oven is used, there is no need to adjust so accurate. It already helps a lot if the raw TC comes down from some 50 ppm/K to maybe 5 or 10 ppm/K. This lowers the requirements on the oven (and the temperature related resistors) by a factor of 5 or 10.  However the problem is that the sensitivity to R1 is higher than the sensitivity to the other resistors of the LTZ1000 circuit.

[iMo]

Random +/-5ppm resistors and the Vref.
The top pane shows the three TCs used (for a doublecheck only).

For each TEMP sweep is generated a random TC coefficient (-5ppm..+5ppm) for each resistor.

The LTspice's random(x) function is something I still do not understand fully  ..

[imisaac]

Yes, imo. The voltage reference sensitivity to the resistor R2 should also be checked as you have done here.

I extracted the R2 sensitivity coefficient manually and plotted it together with the other two coefficients (attached plot).

Surprisingly, the sensitivity coefficients of R1 and R2 have opposite sign and are roughly equal to each other in magnitude.

Generally speaking, is it possible to find two resistors that have equal and opposite tempco and aging effect?

If so, they would be the perfect pair for this circuit.

[Andreas]

The noise is not only a little higher but more like a factor of 100.

Hello,

I have different measurements.
https://www.eevblog.com/forum/metrology/ultra-low-noise-reference-2dw232-2dw233-2dw23x/msg2207748/#msg2207748

Even a cheap SMD Zener in plastic package has only ~2uVpp 1/f noise.

Ok it mainly depends on zener voltage and current.
The lowest noise is usually around 5-6V for the zener and high current.

with best regards

Andreas

[3roomlab]

this is my "scratch pad" simulation of a BJT with -2mv/C (-200mv/100C ?), and a diode with +50ppm/C (for vbr around 6.4v = + approx 32mv over +100C ?)
I think there should be a curve, but I do not know what the curve should look like, so I made it more linear
the BJT tempco parameter appears to be XTB (in my case, its -2.3, used on a 2N2222)
the diode tempco parameter are TRS1 and TRS2 (in my case,  its TRS1 approx=  -0.255, TRS2 1n)
TRS2 controls the quadratic curve fit.
TRS1 controls the linear slope fit.

the original BJT 2N2222 with XTB =1 default does not include a XTB parameter, it appear to fit around -1.5mv/C. if this is default, then all default BJT spice models are not "fitting" 2mv/C. maybe I am missing some other theory, else then, what I found here should be true? (I tried with a mmbt3904, it is nearer to 2mv/C than 2N2222 in fit, mmbt3904 XTB = 1.5 by default model, not 1)

the above require user to edit the dio and bjt files in "cmp" directory.

putting the 2 back into the same .op run from 25C to 125C, produces something that looks like -600ppm/C overall ref circuit, no heater of course. but was it suppose to be -600ppm? is this right?
by modifying the TRS1 to around -0.155. I could then get the bowed curve in the 2nd picture. the curve then becomes manipulated by a pre bias resistor {rt}. I think this part is discussed in the LTZ pdf, unheated compensation? I have seen some online docus talking about this, the curve is not suppose to be bowed but a "s" curve (^3) .

Im not sure if the BJT should be constant current fed or constant voltage
so maybe someone else can improve the model further with a known curve fit.

[Kleinstein]

The zener TC depends very much on the voltage, current and to some degree on the design.

For the BJT a reasonable good approximation is to assume an about linear TC and VBE to extrapolate to some 1.2 V at 0 K. So the higher VBE the less TC and if one starts at some 600 mV at 300 K would get the rule of thumb -2 mV/K.
There is a little curvature in the TC curves, but I would not be so sure the BJT / Zener models are correct on this.

For the zener noise, it depends on the types - the ones I measured so far (in glass) and most datasheets I found where quite horrible. The 2DW232 zener is a rather special low noise type. I don't know if there are other low noise types that really deserve that name.

[3roomlab]

found it
https://www.geosci-instrum-method-data-syst.net/6/301/2017/gi-6-301-2017.pdf
the docu that I saw about unheated compensation
very interesting docu, but it apprears to be part of some huge report over 300-400 pages

[iMo]

With Rb=15k.
PS: I do not see an effect of the PTAT resistor R5 (from that pdf) above, however..

[3roomlab]

I cannot remember if I tried to simulate this, but they have got an extra R5. and in order for the response to be correct (like a ^3-ish curve), the quadratic curve in the diode needs to be accurate/populated, which ... nobody knows whats the value is, so my estimate is just to fit a line, but in real life is suppose to be a curve. it will need a dozen ^ dozen "if then or else steppings" for sure.

** did you try to tempco curve/line fit your diode/bjt? (aka xtb + trs1 ?)

[iMo]

FYI - VBe TCs of some transistors from the lib.

-1,9mV/C in average, except the ON model.

[imisaac]

Here is some complementary information.

In Fig. 3 of the wonderful paper that 3roomlab cited, there is a base resistor rb=15 kΩ added that can correct the circuit tempco at the two temperature extrema (for better agreement between the simulation and the measurement data).

If we assume the choice of the base resistor value is independent to all the other components, then we can again derive the sensitivity coefficients.

It turns out that the base resistor has a negligible effect on the sensitivity coefficients of all the other resistors in the circuit.

Last but not least, there is an additional resistor from the collector to Gnd ("R5" in the paper figure). I feel that it behaves similar to the "R3" collector resistor here (perhaps with a positive tempco effect instead) and therefore may not be worthy to simulate its influence in full.

[imisaac]

FYI - VBe TCs of some transistors from the lib.

I think there are two buried transistors that come with the LTZ1000 TO-5 metal can package. Their tempcos are unknown. However, since they are buried, they may have low tempcos than usual.

[3roomlab]

in this simulation, I put in TRS2= 0.5m for the LTZ. with this curve, you can now get a "flat zone"
finding/characterizing a LTZ with a TRS2=0.5m will be another rabbit hole
but bouncing to a CERN paper which I spoke about in another thread on hpm7717, they are designing a TEC box which completely takes out the variable "external temperature factors". if memory serves, there was a laser hologram nut in here who did his TEC to 1milli celcius accuracy. I think this pretty much ignores tempco and brute forces the box into a temperature compliance.

[imisaac]

Thanks 3roomlab for the revised circuits and the references.

I have a few questions:

1. Regarding the Δ1 mK thermal electric cooler, I think you may be referring to this TEC design here?
http://hololaser.kwaoo.me/electronics/Arduino_TEC/Arduino-TEC.html

2. Regarding the CERN paper, could you provide a reference?

3. Is the voltage reference output in your circuit at the output point of the resistor R10?

[Kleinstein]

Here is some complementary information.

In Fig. 3 of the wonderful paper that 3roomlab cited, there is a base resistor rb=15 kΩ added that can correct the circuit tempco at the two temperature extrema (for better agreement between the simulation and the measurement data).
..

The rb is needed to match the simulations to the real LTZ1000. This resistance may be part of the real LTZ1000 chip - however there may also be just slightly different parameters for the real transistors / zener. Some internal base resistance is normal and this could also have quite some TC. Anyway there is no way to adjust rb. 

The extra R5 reduces the gain of the transistor stage. So it makes the OP (noise and offset drift) a little more important.

AFIAK the transistors are not that special and the main effect on the TC is due to the absolute value of VB: a low VB gives a larger temperature effect.

[3roomlab]

Thanks 3roomlab for the revised circuits and the references.

I have a few questions:

1. Regarding the Δ1 mK thermal electric cooler, I think you may be referring to this TEC design here?
http://hololaser.kwaoo.me/electronics/Arduino_TEC/Arduino-TEC.html

2. Regarding the CERN paper, could you provide a reference?

3. Is the voltage reference output in your circuit at the output point of the resistor R10?

1) I think thats the one, I think it might be possible to use full analog w/o arduino
2) see pdf
3) you mean R12

[iMo]

@3roomlab: the Q3 is within the control loop, afaik, so it does nothing..
Does that Scurve come from your TRS1/2?

PS: the HPM-7177 project looks like a wish list only.. the repo is empty..

[3roomlab]

@3roomlab: the Q3 is withing the control loop afaik, so it does nothing..
Does that Scurve come from your TRS1/2?

TRS2 = 0.5m, try it

for hpm7177, I think tempco = zero is a big deal

[iMo]

Added TRS2=0.5m but I see no change..

[iMo]

Ok, it looks like you must define both TRS1 and TRS2.
Tried below.

PS: BTW, 0.04ppm/C (box) the best result below

[imisaac]

Thanks, imo. The tempco is indeed impressively suppressed.

A couple more questions arise:

1. Are TRS1 and TRS2 user adjustable parameters in the real circuit (via a resistor in series..etc)? Or they are only used in the simulation for a better measurement data and simulation results agreement?

2. I suppose that the output buffer transistor would help reducing the load influence on the voltage reference output. However, shouldn't the tempco of the buffer resistor ("R5" in your circuit) contribute to the overall tempco as well? In that case, I think its contribution would be even stronger than the R1 and R2. 

[Kleinstein]

The Resistors and the transistor for the output buffer after the OP have essentially no influence. They are inside the control loop and thus there change. The series resistance might be needed for the simulation to start.

I don't think one can change the TRS parameters.