Shunt voltage reference in feedback of integrator/opamp?

Thread Starter

Angakok Thoth

Joined Sep 5, 2016
16
I have a common inverting integrators made using opamp (capacitor in negative feedback, +input to GND). I would like to have all these integrators saturate at the same exact voltage. Adding a zener diode in parallel to the cap works, but zeners are 2% tolerance at best and temperature dependent, and i need to make it better than that.

I wonder if I can use Shunt voltage Reference as a precision zener in this kind of circuit. I only seen shunt references used in voltage divider circuits (which they are meant for) and I am unsure, if they would also work in integrators/opamp's feedback. (their current rating isn't a problem. I checked that already)

Also, does anybody know, how good/bad is typically their forward voltage tolerance? It mentioned in datasheets and I would like the . Is it usually at least approximately on par with their reverse voltage breakdown tolerance?

Some people will probably suggest using a rail-to-rail opamps and supplying them with my reference voltages, so they would saturate there. My problem is, that modern rail-to-rail opamps do also have ESD protection diodes, which are causing glitches when used as integrator or comparator. With zener/shunt_ref in feedback, I wouldn't need modern rail-to-rail opamp and could just an old one from times, where ESD diodes were not a thing. (tl072 for example). I know about opa192 being without diodes and being rail-to-rail, but it's expensive and wouldn't work as the smallest supply voltage is 4.5V while my reference/supply voltages would be 3.3V and -0.66V, which is less.

I wish that ESD diodes yes/no would be a parameter I could use for filtering opamps somewhere. I don't think it's humanly possible to look into every r-r opamp's datasheet just to see if it has diodes and if it swings close to rails enough.
 

OBW0549

Joined Mar 2, 2015
3,306
The problem with using a shunt reference for this job is that they typically begin conducting at a voltage much lower than their design reference voltage. The popular TL431, for example, begins conducting at about 1 volt and doesn't reach its design voltage of 2.50 volts until about 400 μA is put through it:

TL431.png

The result is very sloppy (i.e., unpredictable) clamping operation for low integrator input currents.
 

MrAl

Joined Jun 17, 2014
7,500
I have a common inverting integrators made using opamp (capacitor in negative feedback, +input to GND). I would like to have all these integrators saturate at the same exact voltage. Adding a zener diode in parallel to the cap works, but zeners are 2% tolerance at best and temperature dependent, and i need to make it better than that.

I wonder if I can use Shunt voltage Reference as a precision zener in this kind of circuit. I only seen shunt references used in voltage divider circuits (which they are meant for) and I am unsure, if they would also work in integrators/opamp's feedback. (their current rating isn't a problem. I checked that already)

Also, does anybody know, how good/bad is typically their forward voltage tolerance? It mentioned in datasheets and I would like the . Is it usually at least approximately on par with their reverse voltage breakdown tolerance?

Some people will probably suggest using a rail-to-rail opamps and supplying them with my reference voltages, so they would saturate there. My problem is, that modern rail-to-rail opamps do also have ESD protection diodes, which are causing glitches when used as integrator or comparator. With zener/shunt_ref in feedback, I wouldn't need modern rail-to-rail opamp and could just an old one from times, where ESD diodes were not a thing. (tl072 for example). I know about opa192 being without diodes and being rail-to-rail, but it's expensive and wouldn't work as the smallest supply voltage is 4.5V while my reference/supply voltages would be 3.3V and -0.66V, which is less.

I wish that ESD diodes yes/no would be a parameter I could use for filtering opamps somewhere. I don't think it's humanly possible to look into every r-r opamp's datasheet just to see if it has diodes and if it swings close to rails enough.
Hi,

You might be better off connecting a shunt regulator to the output of the op am, with a series resistor maybe 100 ohms or something like that. That way current though the regulator is less of a concern. If you need a buffer on the output, so be it.
 

crutschow

Joined Mar 14, 2008
24,730
Here's the LTspice simulation of an accurate clamp circuit that you could put at the integrator output.
Perhaps some variation of that will work for you.

1584387221560.png
 

Thread Starter

Angakok Thoth

Joined Sep 5, 2016
16
an accurate clamp circuit that you could put at the integrator output.
You might be better off connecting a shunt regulator to the output of the op am,
Thanks, but I need those integrators to saturate at such voltage, so that when I flip the polarity of the current which goes into integrator, then the output voltage will start falling (or rising) immediately. With your solutions, haveing integrator saturate at 5V for example while clamping or shunting it to 3.3V later, then after flipping polarity of the of integrator current , the integrator output would start falling from 5V immediately, but my clamped output voltage would be constant 3.3V for quite a while, until the integrator voltage fallen to 3.3V. I need my output to have precision min & max, but I also need it reacting to the currents going into integrator immediately.
 

MrAl

Joined Jun 17, 2014
7,500
Thanks, but I need those integrators to saturate at such voltage, so that when I flip the polarity of the current which goes into integrator, then the output voltage will start falling (or rising) immediately. With your solutions, haveing integrator saturate at 5V for example while clamping or shunting it to 3.3V later, then after flipping polarity of the of integrator current , the integrator output would start falling from 5V immediately, but my clamped output voltage would be constant 3.3V for quite a while, until the integrator voltage fallen to 3.3V. I need my output to have precision min & max, but I also need it reacting to the currents going into integrator immediately.

Hi,

Ok that makes this more clear.

This may end up a little more complicated, how complicated are you willing to to with this?
Like a couple more op amps maybe?

But if you use the clamp i suggested you might be able to run the cap off of the clamp rather than off of the very output of the op amp. That might make the series resistor very small also so the integration still performs well.
 

Attachments

Last edited:

crutschow

Joined Mar 14, 2008
24,730
if you use the clamp i suggested you might be able to run the cap off of the clamp rather than off of the very output of the op amp.
The problem is that you still get integrator wind-up since the input is still putting current into the capacitor after the output is clamped.

Below is the LTspice simulation of a circuit that clamps the input to stop the integration at the V1 clamp voltage.
The circuit will then hold the output at 3.3V until the input goes positive, causing the integrator output to go lower.
This will allow each integrator to be clamped to the exact same voltage.
R4 and C2 are to stabilize the loop.

1584420725918.png
 
Last edited:

Thread Starter

Angakok Thoth

Joined Sep 5, 2016
16
R4 and C2 are to stabilize the loop.
You're a genius. Testing it also in LTSpice. Now my only problem is, that that R4 and C2 make it too slow for my application and I'm getting overshoots before it settles at the reference voltage. Different values seem to make it work better, but how do I check the stability? Sometimes the plot looks alright unless I zoom in. Sometimes I guess stability issues when it takes 20x longer for spice to compute. What's the proper method the check it?
 

MrAl

Joined Jun 17, 2014
7,500
Hello again,

Here is another version that is very fast and with very little overshoot.
The two 10 ohm resistors can be shorted out if a little bit more overshoot is acceptable, although it is still low.
Just to note, transistors have been used in the feedback section of integrators like that for a long time. Sometimes they are used like that to reset the capacitor after an integration cycle to get it ready for the next measurement.
 

Attachments

crutschow

Joined Mar 14, 2008
24,730
What's the proper method the check it?
You just look at the settling times of both U1's and U2"s output to see if it meets your requirement and that there is no significant overshoot or ringing in either signal.

It's difficult to suggest solutions when you haven't stated the operating requirements.
What is your highest frequency requirement, what is the nature of the integrator input waveform, and what is the integration time constant you have?
You may need to use a faster op amp.
 
Last edited:

Thread Starter

Angakok Thoth

Joined Sep 5, 2016
16
You just look at the settling times of both U1's and U2"s output to see if it meets your requirement and that there is no significant overshoot or ringing in either signal.
It's difficult to suggest solutions when you haven't stated the operating requirements.
What is your highest frequency requirement, what is the nature of the integrator input waveform, and what is the integration time constant you have?
You may need to use a faster op amp.
Thanks for your reply. This may be difficult, as I need to allow relatively wide range or speeds.
To allow that, I am driving the integrator from a variable current source (voltage controlled in exponential manner, so huge range is allowed comfortably).
Integrator's input waveform is a squarewave (derived from cmos logic, but later filtered with 10KHz 1-pole lowpass). Flipping between + and -.
If it's possible, I would like to allow times (of integrator output getting from 0V to 3.3V or backwards) around 100us to 1s if posible. That's 4 orders of magnitude.
If impossible, then at least 330us to 330ms, which is still 3 orders of magnitude.
To achieve that, I can use any section of the current source's range, which is 10nA to 3mA.
For timing caps, I'll be using quality film caps and would like them to be 100nF or smaller if possible.

Now if it was setting just 1-2 values by trial and error, I would just brute force it with step param and choose.
But there are 3 parts in the stabilizing part, and that would be a lot of possible combinations even if LTspice allowed more than 2 ".step param"s.

Maybe a deeper understanding would allow using just two parameters to define those three C2, R3, R4 values?

For example if it wasn't the absolute values of the three parts what's really important, but rather some two constants, like for example (this probably incorrect)
R3:R4 ratio is important, as it's an important factor for determining voltage at negative input pin.
C2 * (R3 + R3) is important, as it defines how fast will the C2 capacitor charge from the voltage at integrator output.

Then I could step param those two things, and define the parts parametrically. (two of them, while the 3rd one would be fixed to something reasonable, to make them all withing reasonable 1K-1Meg and 100p to 1u range).

The steps which lack stability take crazy long to compute, but I would just run it before going to bed and then choose.
But I need to find a way to reduce the define those 3 values using just 2 parameters.
(or learn a different spice, where 3 params are possible).
 
Last edited:

MrAl

Joined Jun 17, 2014
7,500
Thanks for your reply. This may be difficult, as I need to allow relatively wide range or speeds.
To allow that, I am driving the integrator from a variable current source (voltage controlled in exponential manner, so huge range is allowed comfortably).
Integrator's input waveform is a squarewave (derived from cmos logic). Flipping between + and -.
If it's possible, I would like to allow times (of integrator output getting from 0V to 3.3V or backwards) around 100us to 1s if posible. That's 4 orders of magnitude.
If impossible, then at least 330us to 330ms, which is still 3 orders of magnitude.
To achieve that, I can use any section of the current source's range, which is 10nA to 3mA.
For timing caps, I'll be using quality film caps and would like them to be 100nF or smaller if possible.

Now if it was setting just 1-2 values by trial and error, I would just brute force it with step param and choose.
But there are 3 parts in the stabilizing part, and that would be a lot of possible combinations even if LTspice allowed more than 2 ".step param"s.

Maybe a deeper understanding would allow using just two parameters to define those three C2, R3, R4 values?

For example if it wasn't the absolute values of the three parts what's really important, but rather some two constants, like for example (this probably incorrect)
R3:R4 ratio is important, as it's an important factor for determining voltage at negative input pin.
C2 * (R3 + R3) is important, as it defines how fast will the C2 capacitor charge from the voltage at integrator output.

Then I could step param those two things, and define the parts parametrically. (two of them, while the 3rd one would be fixed to something reasonable, to make them all withing reasonable 1K-1Meg and 100p to 1u range).

The steps which lack stability take crazy long to compute, but I would just run it before going to bed and then choose.
But I need to find a way to reduce the define those 3 values using just 2 parameters.
(or learn a different spice, where 3 params are possible).
Hi,

When you run into very long sim times that is the time to jump into a full blown circuit analysis which can tell you a lot about the performance of a circuit and allows you to compute outputs for very unusual input waveforms much much faster than with a simulator.

Since Cruts' design is non linear because of the diode, and because of the way the associated op amp behaves, you can linearize it by replacing the diode with a resistor of an appropriate value and get a very similar response. The value should be 20k or less which is the value of the input resistor. In fact, you can replace the diode with that resistor in the actual circuit also and keep the whole thing linear.
The response is then probably 2nd order overdamped but we can look into this if you like.
The approach then is most likely convolution in one domain or another or piecewise convolution in the time domain which is still a very fast method of analysis.

If you show some of your input waves i can show you the frequency domain equivalents or suggest another way to handle them without using a simulator and therefore get very fast results. The time response for a 2nd order system is very easy to compute.
To show your input waves draw a diagram and label the time and amplitude at the key points.
 
Last edited:

Thread Starter

Angakok Thoth

Joined Sep 5, 2016
16
If you show some of your input waves i can show you the frequency domain equivalents or suggest another way to handle them without using a simulator and therefore get very fast results. The time response for a 2nd order system is very easy to compute.
To show your input waves draw a diagram and label the time and amplitude at the key points.
Thanks, well my input current waveform has edges which are not too sharp (10KHz 1st order low pass filtered). And those edges are between parts of constant values (currents) between 100nA and 1mA, and of either polarity, and they last for at least 100ms.

So I could perhaps consider something like this sequence +1mA, -1mA, +100nA, -100nA, each step lasting 5 seconds for example.
 

MrAl

Joined Jun 17, 2014
7,500
Thanks, well my input current waveform has edges which are not too sharp (10KHz 1st order low pass filtered). And those edges are between parts of constant values (currents) between 100nA and 1mA, and of either polarity, and they last for at least 100ms.

So I could perhaps consider something like this sequence +1mA, -1mA, +100nA, -100nA, each step lasting 5 seconds for example.
Hi,

Oh ok, well that would be simple to calculate, but i cant imagine the simulator taking too long either maybe we could look into that in itself.

But it is good that you define these inputs because i was assuming you had a unipolar signal. Now i can see that the input is bipolar. But what about the output? I assume you want to clamp at 3v or 3.3v, but do you also need to clamp at -3v or -3.3v too?


And this is a current not a voltage? That requires a slightly different input part of the circuit then.
 

Thread Starter

Angakok Thoth

Joined Sep 5, 2016
16
I assume you want to clamp at 3v or 3.3v, but do you also need to clamp at -3v or -3.3v too?
And this is a current not a voltage? That requires a slightly different input part of the circuit then.
I clamp the integrator at -0.33 and +3.3.
As I mentioned, I am driving the integrator from a current source. It shouldn't be much different from driving integrator from variable voltage through a fixed resistor - also gives a variable current.
This is what it looks like:
clamped_integrator.png
 

MrAl

Joined Jun 17, 2014
7,500
I clamp the integrator at -0.33 and +3.3.
As I mentioned, I am driving the integrator from a current source. It shouldn't be much different from driving integrator from variable voltage through a fixed resistor - also gives a variable current.
This is what it looks like:
View attachment 201892
Is that the circuit that is taking a long time to run through in time domain analysis in LT Spice?
Why dont you post the asc file so we can take a look too.
Looks ok though, but seeing the simulation work would help.
 

crutschow

Joined Mar 14, 2008
24,730
In you post #16 circuit, with only a positive current input, the integrator output can only go negative, never positive.
How will you reset the integrator or make it go positive?
 

Thread Starter

Angakok Thoth

Joined Sep 5, 2016
16
In you post #16 circuit, with only a positive current input, the integrator output can only go negative, never positive.
How will you reset the integrator or make it go positive?
it's not only positive... I probably shouldn't have drawn that arrow there, but as written there: +-100nA to +-1mA.
 

crutschow

Joined Mar 14, 2008
24,730
it's not only positive... I probably shouldn't have drawn that arrow there, but as written there: +-100nA to +-1mA.
How "stiff" is the constant current source?
Can it be used to directly charge (Integrate) the capacitor to 3V, thus avoiding the frequency response requirement of an integrator op amp?

Can the capacitor value be switched on-the-fly to cover the wide integration values?
 
Last edited:
Top