Continue to Site

Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

Register Log in

[SOLVED] This zener diode is not working as it should work

Status
Not open for further replies.
F

flote21

Advanced Member level 1
Joined
Jan 22, 2014
Messages
411
Helped
1
Reputation
2
Reaction score
3
Trophy points
1,298
Activity points
5,595
Hello guys!

I am wondering about a simulation in LTSPICE with the Zener diode: BZT52C3V0T-7

I have downloaded the Spice model from the manufacturer website: https://www.diodes.com/part/view/BZT52C3V0T

And I have run a simulation of two cases:

1) Case 1 with R1=150Ohm

R1-150Ohm.png

2) Case 2 with R1=0Ohm

R1-0Ohm.png


The case 1 looks ok for me because VZ=3.29V and the Zener is working fine. But the case 2 it does not make sense because Vz=5V and according to the manufacturer, it should be limited to Vz(3V therotically). This issue is also happening when you replace V1 by a OpAmp like this:`

OpAmp.png

Anyone could explain what is happening?

Thanks in advance!
 

The current in the Case 2 is too high so the model is not valid anymore.Every model has a validity region in simulations.They are mathematical expressions with constraints and they represent the component in a limited OP region
Case 1 is correct biasing..
 

Hi flote21,

you need some series component at which the voltage difference V_diff = V1 - VZ drops, i.e. a resistor where the voltage difference of 2 V is applied.
Choose the value of R1 in accordence with the stated test current I_ZT in the datasheet (I_ZT = 5 mA) and the current which is sinked by your load (I_L = V_Z / R2 = 3 V/ 1 kΩ = 3 mA).
--> R1 = V_diff / (I_ZT + I_L) = 2 V / (0.005 A + 0.003 A) = 250 Ω.

By doing so, you should gain your desired VZ of 3 V.

Greets
 

Hi!

The case 2 is clear for me now. But what's up with the OpAmp case. According to the OpAmp manufacturer its output current is limited, and I have measured the dropcurrent at the Zener and it is 23mA. So the Vz=3V and in the simulations Vz=5V.

Greetings
 

Hi,

you also need a series resistor for the opamp implementation, as the opamp regulates its output in such a manner to bring the difference between its inputs is zero. Consequently, its output voltage is 5 V.
Unless you are not using a current source instead of a voltage source, you need some kind of length/series element where your aimed voltage difference of 2 V drops. This can be a resistor or even 3 ordinary diodes (3 • 0.6 ... 0.7V = 1.8 V ... 2.1V).

BR

- - - Updated - - -

... further the used opamp is able to drive a load with a current up to ±54 mA (@ Vs = ±5 V), so you can expect that the opamp output voltage does not decrease/collapse for a current of 23 mA, and stays at 5 V.
 
Apparently Onsemi has engaged first year students to write SPICE models. Check the model I/V characteristic against the datasheet and realize that it's just garbage.
 
If in real life you connect a 3V zener to a 5V source, the magic smoke would come out from somewhere.
 
schmitt trigger said:
If in real life you connect a 3V zener to a 5V source, the magic smoke would come out from somewhere.
Click to expand...

I agree with that. Imagine an automotive battery with 12 V (yes the heavy bulky lead battery ;-)) connected to a Z-diode with a rated break down voltage of 10 V (to be consistent with the desired voltage difference). You would't expect an 2 V decrease of the battery, the battery holds its 12 V and blows your diode.

Further, the AD8510 is a driven source, so if it sources 23 mA and you expect a voltage at the Z-diode of 3 V, that could only be caused by the output impedance of the opamp itself. So for your example the opamp would "need" an output impedance of ~87 Ω (2 V/0.023 A). Luckily it has a low impedance (as desired). By having a look at Fig. 22 in the datasheet an output impedance of maybe 1 Ω can be assumed (if at all).

BR
 
Hi guys!!

Thanks for your replies! I understand now what is happening with the opamp case.

BR
 

Luckily it has a low impedance (as desired). By having a look at Fig. 22 in the datasheet an output impedance of maybe 1 Ω can be assumed (if at all).
Click to expand...
Datasheet output impedance is a small signal quantity and not relevant in this situation. Instead you'll look at large signal output characteristic respectively output current limiting. 40 or 50 mA sourced by the OP might overheat the zener diode, but not raise the diode voltage to 5V according to datasheet. It's an incorrect model.
 
  • Like
Reactions: stenzer

    stenzer

    stenzer

    Points: 2
    Helpful Answer Positive Rating
FvM said:
Datasheet output impedance is a small signal quantity and not relevant in this situation.
Click to expand...

Thank you for pointing that out! I overlooked the input voltage stated with 50 mV in Fig. 22.

FvM said:
40 or 50 mA sourced by the OP might overheat the zener diode, but not raise the diode voltage to 5V according to datasheet. It's an incorrect model.
Click to expand...

Ok, I see your point. If the model would be correct, the opamp wouldn't be able to regulate its inpt difference to zero (I/V relation is far to steep), thus leading to a Vz of 3 V.
You caught me on the wrong foot :wink:. Thank you for clarifying that!

greets!
 

Therefore according to the datasheet of the f
Diode, with Rs=Oohm, Vz=3V with Vin_OpAmp=5V. Right?
 

Therefore according to the datasheet of the f
Diode, with Rs=Oohm, Vz=3V with Vin_OpAmp=5V. Right?
Click to expand...
No, diode voltage is about 4V at the expected 50 - 60 mA OP short circuit current. OP and zener diode will run quite hot, but still work inside their power rating.

Why would you operate a zener diode this way?
 
FvM said:
No, diode voltage is about 4V at the expected 50 - 60 mA OP short circuit current. OP and zener diode will run quite hot, but still work inside their power rating.

Why would you operate a zener diode this way?
Click to expand...

Hi!

i wanted to operate the diode without the current limit resistor to avoid a drop voltage of the zener at the ADC input.

Thanks anyway for all your answers.

Greetings
 

i wanted to operate the diode without the current limit resistor to avoid a drop voltage of the zener at the ADC input.
Click to expand...
Doesn't make sense. If the OP has decent current limiting, OP and zener diode will hopefully survive. But the clamp voltage is considerably higher, hence the apparently intended ADC protection isn't achieved.
 
Hi!

We have tested in the lab and the output current of the OpAmp is 17mA when the zener resistor is 0Ohm. So it is far away of the max. output current of the opamp.

Furthermore, the clamp voltage of the diode is higher than the max input voltage of the ADC. But according to the test I made in the lab, when the zener resistor is higher than 5Ohm, the zener diode starts a desviation of the opAmp output voltage at 2.1V. I would like to have not any desviation of the output voltage at the ADC input range: 0<=Vin_ADC<=2.5V.

Greetings
 

Simulations are not real, instead they use magic. Many transistors and opamps can be extremely overloaded but in a simulation they work fine.
 

flote21 said:
I would like to have not any desviation of the output voltage at the ADC input range: 0<=Vin_ADC<=2.5V.
Click to expand...

What is your planed application?
How does the input signal applied to the ADC look like?
Why should the input voltage applied to your ADC should not change?

What kind of signal should the ADC sample? It makes no sense to me if the output voltage (of the AD8510) at the input of the ADC should not deviate, so there will be no information provided at all, except a single voltage value. But as you mentioned, as it the input signal should be "stable", there would not be the need of an ADC to observe this voltage.

Should the ADC be used to observe a reference voltage?

If the intended usage has a protective purpose, there are other ways to realize that i.e. two schottkey diodes reverse operated, one with its cathode connected to VDD and the anode to the ADC input. The other diode's cathode is connetced to the ADC input and the anode to system ground, see [1].

[1] https://www.analog.com/en/technical-articles/protecting-adc-inputs.html

greets
 
  • Like
Reactions: FvM

    FvM

    FvM

    Points: 2
    Helpful Answer Positive Rating
when the zener resistor is higher than 5Ohm, the zener diode starts a desviation of the opAmp output voltage at 2.1V
Click to expand...
As previously mentioned zener diodes don't provide selective input protection. This also includes considerable leakage current below the nominal zener voltage. Schottky diodes as suggested by stenzer may be a solution. But they also involve leakage and clamping overvoltage at higher currents, in addition unwanted capacitance for high speed applications. Consider that many modern ICs have substrate diodes rated for continuous 5 or even 10 mA that can act as overvoltage clamp with current limited sources. In many cases a rail-to-rail amplifier powered by the same supply as the ADC is however the best solution.
 

Status
Not open for further replies.

Similar threads

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Back
Top