ADR1399 Datasheet

[razor6271]

Hi,
I have been trying to replicate the ADR1399 datasheet graphs under "typical performance characteristics" for my research on LTSpice, but I have been facing two issues:
a. On using the circuit under "Theory Of Operation" (Pg. 12) for the 4-Pin TO-46 package, I am unable to get similar characteristics in LTSpice, because a lot of things are unclear in the circuit in comparison to the parameters given on the graphs.
b. I am not even sure if this is the correct test circuit to get the same readings as those graphs and I am unable to find anything different to try.
I have attached an example of what I was getting and what the graph showed, so please let me know if I am doing something completely dumb, would appreciate any suggestions.

 

[FvM]

What do you expect to see in your simulation? I presume heater effect isn't modelled at all in the simulation component.

 

[razor6271]

What do you expect to see in your simulation? I presume heater effect isn't modelled at all in the simulation component.

https://www.analog.com/media/en/technical-documentation/data-sheets/adr1399.pdf

I want to see :
a) Heater Current vs Time
b) Response time effect due to Rcomp and Ccomp
c) Effect of temperature on reference voltage
d) Voltage noise
The graphs in LTSpice should match those in the datasheets which I can't seem to match

 

[FvM]

a) don't expect that time behaviour of heater circuit is modelled.
b) You don't see transient waveforms because you don't have any time variant stimulus, e.g. pulse source. You can however visualize power-on transient by selecting "skip initial transient solution" option.
c) Not sure if t.c. is modelled, heater most likely isn't. You can try .temp statement to check for static t.c.
d) SPICE doesn't model semiconductor noise in transient analysis

 

[razor6271]

are

a) don't expect that time behaviour of heater circuit is modelled.
b) You don't see transient waveforms because you don't have any time variant stimulus, e.g. pulse source. You can however visualize power-on transient by selecting "skip initial transient solution" option.
c) Not sure if t.c. is modelled, heater most likely isn't. You can try .temp statement to check for static t.c.
d) SPICE doesn't model semiconductor noise in transient analysis

Are there any graphs I can get in ltspice other than these from the datasheets? I am not very sure about the limitations of Spice.
Thank you!

 

[D.A.(Tony)Stewart]

Left is the internal Test diag.

 

[razor6271]

View attachment 192178
Left is the internal Test diag.

Thank You.
I just wanted to ask if there are any ways I can model the IC so it shows variation with temperature too. Because it's an important part of why I chose ADR1399 for my research and I need to show it's response to temperature.

 

[FvM]

You can test ADR1399 model behaviour to understand which properties are included.

What I see so far:
- models static behaviour of heater circuit, including temp dependency, similar to datasheet figure 10. Behaviour below 10 V input looks erroneous.
- models typical tempco of zener voltage with nominal regulated steady state temperature
- does not model relation between heater and reference

In so far, your expectation to get info from simulation not contained in the datasheet is in vain.

In older days, manufacturers used to specify which properties of a part are SPICE modelled and which not. The ADR1399 LTspice black box model is apparently a roughly simplified behavioral model. You better refer to datasheet specs and derive behaviour mpodels on your own, if you need it.

An important parameter, unregulated zener tempco, is missing in ADR1399 datasheet. Suggest to refer to other buried zener devices like ADR1000 or ADR1001 to get an idea about it.

 

[7f6grenade]

So, if I am correct. is this missing zener the same one that takes away the effect temperature has on reference voltage ? If yes. are there are any ways for me to incorporate this Zener with the ADR1399 so I can show that I am getting a difference of 7.05V across a large temp range?

 

[D.A.(Tony)Stewart]

The datasheet should answer most of your questions except your plot discrepancies.

If the specs or test results do not meet your expectations, there may be a difference in setup.
If thermal stability is an issue, look for gradient issues like a ground plane on one pin. They test in a socket which offers some thermal isolation from the PCB.

Isolation from thermal gradients with added insulation will reduce thermal errors, such as a few mm of ESD styrofoam. That will result in a lower temperature coefficient if the gradient is reduced. **

If your results do not meet expectations, the ADR1000 or ADR1001 design is much better for short-term stability and aging. These have the same temperature coefficient as the ADR1399 and will be reduced with the above ** attention.

The forced air inside a thermal chamber may disturb the case temp and stability.

Please show how you tested your major concern and deviation from the plot.

 

[razor6271]

The datasheet should answer most of your questions except your plot discrepancies.

If the specs or test results do not meet your expectations, there may be a difference in setup.
If thermal stability is an issue, look for gradient issues like a ground plane on one pin. They test in a socket which offers some thermal isolation from the PCB.

Isolation from thermal gradients with added insulation will reduce thermal errors, such as a few mm of ESD styrofoam. That will result in a lower temperature coefficient if the gradient is reduced. **

If your results do not meet expectations, the ADR1000 or ADR1001 design is much better for short-term stability and aging. These have the same temperature coefficient as the ADR1399 and will be reduced with the above ** attention.

The forced air inside a thermal chamber may disturb the case temp and stability.

Please show how you tested your major concern and deviation from the plot.

Hello, so I did run some tests and what I believe is I have found a bug in the model of ADR1399 that LTSpice provides. According to the diagram in datasheet, the heater side and the reference side are not connected, but according to my test results, it shows that the current that comes in heater+ and Ref+ gets all out from Ref-, i.e no current flows from Heater- , which probably means that in the model they somehow short-circuited the heater side causing erroneous current to flow through the resistor I have connected to ref-. Is there anything I can do about this ?

 

[FvM]

Not a bug, read datasheet thoroughly. Heater- is connected to chip substrate and must be most negative terminal. Maximum ratings specify 0.1 V margin.

Apparently substrate diodes are modelled but thermal connection between heater and zener reference isn't.

 

[razor6271]

Not a bug, read datasheet thoroughly. Heater- is connected to chip substrate and must be most negative terminal. Maximum ratings specify 0.1 V margin.

Apparently substrate diodes are modelled but thermal connection between heater and zener reference isn't.

so, if there is 60mA current flowing in from heater+, there should be the same current or atleast some current at heater-, but I get no current there and all the current gets out from ref-, I am not sure if I am understanding this correctly.

 

[FvM]

You didn't show your simulation circuit, I presumed you are floating Heater-. If not, there's probably a bug. I'll check myself.

 

[razor6271]

You didn't show your simulation circuit, I presumed you are floating Heater-. If not, there's probably a bug. I'll check myself.

Sorry, but the .asc file is attached, I did attach a resistor with heater- to see if any current flows from it but it shows 0mA.

 

[FvM]

You are right, ADR1399H model has incorrect heater return current. I tested ADR1399E up to now, it doesn't have this problem.

--- Updated Jul 14, 2024 ---

Other than guessed, substrate diodes are not modelled.

 

[razor6271]

You are right, ADR1399H model has incorrect heater return current. I tested ADR1399E up to now, it doesn't have this problem.

--- Updated Jul 14, 2024 ---

Other than guessed, substrate diodes are not modelled.

Thank you for the help. I'll try to do something with the E model then if there is no workaround with the problem that the H model has.

 

[FvM]

Just noticed that ADR1399H.sub has more errors. To get correct results, pin 2 and 4 must be both connected to GND (node 0). Parts of the model are apparently reacting on ground shift, most likely they are erroneously using node 0 respectively aboslute voltage reference internally.

See that wrong heater connection is known error https://ez.analog.com/design-tools-...14/possible-bug-with-adr1399-model-in-ltspice

 

[D.A.(Tony)Stewart]

I get almost the same results for suffixes E & H, settling to 7.5 mA on the heater for both models using startup < 50 us. This is not a thermodynamics transient model so don't expect it.

The IC must drive the transistor heater and use the Vbe voltage vs temperature characteristics internally while subtracting any rBE and modulating the current to control the temperature with a 1 ppm fast settling time I would expect in a few seconds to a step disturbance. So insulating the case from disturbances will assist your design. Since the simulation cannot achieve your desired results, you must follow the datasheet design specs and test as required with your objective specs. (TBD)

Sorry about the scales and colours not matched. I loaded them from the library .asc file then added V1=30V with .tran 0 50u 0 startup

Although, I have no experience with this IC, I have thoroughly tested a custom 2oz FPC foil in styrofoam oven for metal can Xtals and achieved < 1 ppm freq. stability in < 10 s using 0603 heater resistors and a thermistor feedback from 25'C to 70 'C.

--- Updated Jul 14, 2024 ---

A bipolar supply for the heater seems to give the same results for me.