Repairing a current-to-voltage preamplifier

[LoveLaika]

This is for an STM?  I used Google to look for "STM transresistance amplifier".  Here's some links off the first page:

https://aip.scitation.org/doi/full/10.1063/5.0011097

https://www.researchgate.net/profile/Emiliano_Pallecchi/publication/234889355_Development_of_an_ultralow_current_amplifier_for_scanning_tunneling_microscopy/links/0046351a838873e8f3000000/Development-of-an-ultralow-current-amplifier-for-scanning-tunneling-microscopy.pdf?origin=publication_detail

https://arxiv.org/pdf/physics/0610280.pdf

Choosing the parts shouldn't be that difficult.  I haven't worked with pico and femto Amp currents, however I expect the bigger problem will be to design and fabricate an assembly that will work.  I would look into design and construction techniques for electrometers.  One thing  done is to lift the summing node components off the circuit board and support them with the minimum number of PTFE standoffs.  Looking at the module in the image above, I see the input is separated from the other pins.  Distance is one way to reduce leakage currents.

I wonder if the original design was done as a hermetically sealed module not only to control leakage currents, but also to control outgassing under vacuum?  I worked on various projects that used multi-watt laser diodes and as we gained experience with building these things found that adhesive outgassing affected long term reliability because it deposited a contaminating layer on the optics.  This was at atmospheric pressure and just above the typical room temperature.  We went to low outgassing products and increased the curing and outgassing times.

Do you know if there are any organic based items in the microscope's vacuum chamber?

Thank you for your reply. Sorry I couldn't get back to you sooner. What do you mean by organic-based items? For what it's worth, I don't believe so, but to be fair, I'm not running the STM experiments. Ideally, in the long run, since this thing isn't manufactured by Omicron anymore, we're trying to build a replacement based on the information above.

[LoveLaika]

Now that sounds like fun

30kHz means 33µs period. For such bandwidth, your feedback network's time constant must be no more than 5µs. With a 100MΩ resistor this is at most 0.05pF capacitance. That's 1/20th of a picofarad, less than some resistors have between their ends.

You probably don't want to increase that resistor to 1GΩ.

Maybe a different question for a change
How did you test the original amplifier? What really is wrong with it?
How will you test the replacement? You may want to verify its frequency response to avoid surprises.

Thanks for your reply. Sorry for not responding sooner. Been busy with other tasks.

Currently in the lab, we have two IVC preamps. One of them broke, and we're using the second one for the time being. To be fair, I'm not doing the STM measurements myself. According to the professor who is doing it, the one that broke was broken because one of the pins broke off. Thus, he used some epoxy in an atteInmpt to use a piece of metal to connect back to the broken tip. While we're not necessarily trying to fix this per se, we are trying to replicate the functionality of this preamp so we don't have to buy it again (Omicron said they don't make this anymore, so they're out).

I honestly haven't tested the preamp myself. I'm just going by what I was given.

[LoveLaika]

The Johnson noise current of the feedback resistor decreases with increasing resistance, so one should use as high a value as possible with low input currents.  The resistor's noise current adds (in quadrature) with the amplifier's input noise current and the amplifier's input noise voltage divided by the total resistance seen at the inverting input.

Thanks for your reply. Sorry for not replying sooner.

Looking at the specs, what bothers me is how the op-amp supposedly gets a gain of 10e8. In this inverting gain config, wouldn't you get a gain of 10k given the resistances? How would you get that 10e8 gain with those resistor values?

Aside from that, the offset voltage is stated to be 500 uV, so assuming I understand what that means, when pins 1 and 2 are unconnected, there's a 500 uV voltage measured between the two if the op-amp is powered? How do you pick the diodes shown in the schematic?

[duak]

I mentioned organic compounds above.  The original preamp looks like it's built into a metal/ceramic package that might even be hermetically sealed.  If I understand how many STMs are put together, the preamp is located within the vacuum chamber and the components are exposed to high vacuum.  Many of the components on the replacement are made of organic materials such as epoxy that may absorb contaminants under atmospheric pressure and outgas under vacuum.  I'm wondering if this might be a problem?

[LoveLaika]

I don't think the preamp was within a chamber or the like. When I saw it, it wasn't in a chamber. It was laying on the top, easily accessible with connectors attached to the pins. If it helps, here's a link that might give you a better idea.

https://groups.google.com/forum/#!searchin/surfacescience/IVC|sort:date/surfacescience/PpgaSCq90lw/JZdzigi4DgAJ

In a nutshell, the current coming from the tip goes into that tiny little preamp which turns it into a voltage. That voltage goes into another preamplifier and another series of amplifiers, which then goes to the computer to be read.

If it helps, my system is a VT STM by Omicron.

[magic]

You suggested that this preamp sits in the vacuum chamber by stating that it sends its output to another amplifier outside the chamber.

Looking at the specs, what bothers me is how the op-amp supposedly gets a gain of 10e8. In this inverting gain config, wouldn't you get a gain of 10k given the resistances? How would you get that 10e8 gain with those resistor values?

Yes, closed loop voltage gain is 10⁴, at least at frequencies where the opamp is fast enough to support it. But that's not the spec they give - it doesn't have a gain of 10⁸ but current-to-voltage conversion ratio of 10⁸. And why wouldn't it? Calculate what current must be fed into the TIP input for the output to deflect by 100mV

Aside from that, the offset voltage is stated to be 500 uV, so assuming I understand what that means, when pins 1 and 2 are unconnected, there's a 500 uV voltage measured between the two if the op-amp is powered? How do you pick the diodes shown in the schematic?

The IO input is high impedance so it needs to be externally driven or else it could drift randomly or slam into one supply rail. Once that is sorted, yes, the TIP will be maintained within ±500µV by cancelling the TIP input current with current through the feedback resistor. That's how those converters work.

[TimFox]

The gain of a transimpedance amplifier (current-to-voltage) has the dimensions of ohms:  this gain would be 10⁸

[LoveLaika]

Thanks. Sorry, I was thinking of the mindset of V-to-V and not I-to-V. The math makes sense now.

If you don't mind me asking, the diodes seem to limit the voltage swing between the two op-amp inputs when there is a current present at TIP, so that way, the two voltages don't have a really big difference between the two inputs. Is this correct?

I did some research and while it doesn't say what diodes are being used, I looked at corresponding circuits involving the same STM, and the preamplifier after that uses a comparator op-amp that has diodes like what is shown in the images in my first post. It uses the BAV45, and judging by the diode description, it may be suitable here given its two forms:

https://my.centralsemi.com/datasheets/BAV45.PDF
https://my.centralsemi.com/datasheets/CPD65-BAV45_WPD.PDF

[LoveLaika]

Thanks. Yeah, I made the mistake of thinking of V-to-V when I should have thought of it as I-to-V. The math makes sense now. Sorry about that.

[LoveLaika]

There are only very few parts in the circuit. Besides the parts shown, they may be a capacitor at the supplies. The 2 diodes could be one part (e.g. BAV199 or similar).

I don't know of any ready made chips with the function, so it would need  the diodes, 2 resistors and the OP.
For just a single unit one may get away with air wiring or a hand carved PCB.

The 100 M resistor may be slightly tricky to find in a small form factor. The parasitic capacitance in parallel to the resistor may be important too, as it effects the bandwidth: to little and the circuit may oscillate, to much and the circuit gets slow. The values depends on the input capacitance and of the OP and the diodes. It may need a few tries to find the right value / OP with suitable speed and capacitance.

I was doing some research regarding this part and the part that it goes to. It's part of an STM. The tip current goes through this IVC and gets converted to a voltage. That voltage goes back into another preamplifier (let's call that one big preamplifier) for more amplification, which then goes back to the computer to be read.

Perhaps it may be meaningless, but I was kind of looking at the circuit ahead, and there's an optional op-amp circuit that was being used. Now, in my 'big preamplifier', option E is not present. Rather, it is bypassed. However, assuming that it is there in some options, I can't help but think that some parts used there that may be used in the IVC, specifically the diodes. The BAV45 is a switching diode, but it's used for picoamps. In this configuration, it seems to limit the voltage difference between the two op-amp inputs, so perhaps it might be used here in the IVC.

[SMdude]

Diodes on the inputs like that clamp the input voltage which helps not saturate the opamp input/output.
If the signals of interest are only tiny then diodes like that work well and block large unwanted signals, allowing the opamp output to settle quickly so the measurement can be taken.
It would be interesting to see scope shots of the receiver output from this device.

[LoveLaika]

Thanks for your reply. Sorry, I don't have scope shots of the device. Only simulation shots. I ran a hypothetical simulation using the OPA602 compared with an ideal op-amp with and without diodes.  You can see the results here. Sorry if it's hard to see.

Assuming that my current-to-voltage op-amp uses the same diodes as in that option E circuit, I sent a pulse of 50 nA to my three circuits to see how they behave. It's just like you said, the diodes effectively limit the input voltage. Otherwise, via my ideal op-amp at INV1, I get a large difference of 5 volts rather than 10 mV with the diodes. I think that this is what I want if I want to keep the potentials between the two inputs close to each other as in the case of my IVC.

[TimFox]

Is this a safety circuit to prevent the probe from coming too close to the sample?

[LoveLaika]

The circuit as a whole? I don't think so, based on the pictures of the manual I posted in the original post. The diodes shown in the original image might be there to make sure that voltage between TIP and I0  don't deviate from one another by a large scale (only by a few millivolts), but I don't know for sure. I0 is supposedly the reference voltage at which TIP is being held against. I believe it is the same with the op-amp. So, from this op-amp's point of view, I0 is effectively 'GROUND'.

[LoveLaika]

@SMdude Sorry for not replying sooner. Been busy with other projects that took over time. Regarding what you said, I see that diodes just clamp the input voltage, but it seems to have an effect on the output signal. Take a look at my SPICE simulation below using the ideal op-amp model. You can see how the different diodes affect the output signal. In each op-amp circuit, I'm using the same current signal, and the op-amp without diodes is used as a control to see how the diodes affect the output.

Doing research, I found that Central Semiconductor's diode, BAV45, is obsolete. Using other common diodes, you can see at the bottom how the output is greatly distorted (at least when compared to the control). Op-amp aside, what diodes would be good replacements for the BAV45? That seems to be the major issue.

[LoveLaika]

So, with the spec of dust info, your probably dealing with an STM.

I put an EBIC system together.  Building the stage was the hard part.  I built a faraday cup, so that the beam current could be measured.

The 100 M resistor is the real pain.

Ib is a critical parameter and Ib varies with temperature which affects Vos.

See: https://www.analog.com/en/products/ada4530-1.html#product-quality

I used the OP41 for one design.  That one is obsolete.  https://www.analog.com/media/en/technical-documentation/obsolete-data-sheets/75599329OP41.pdf

The AD549 is a suggested replacement.

Usually there is a capacitor across the 100 M resistor .   Put the (-) input on a PTFE post.

I'm sorry for replying so late again. Unfortunately, other projects got in the way, and now I'm back to researching this problem again. With your suggestion, how would you go about simulating whether or not the component will work? I tried running a simulation, comparing the AD549 against an ideal op-amp model in SPICE. They all use the same current signal. You can see how the ideal op-amp gives a close to perfect square wave when I convert the current square wave signal to voltage. When compared to the AD549, the AD549 performs rather poorly. I know that it won't match up to an ideal op-amp, but is this the best way to determine whether or not the op-amp will work, or am I testing this in the wrong way?

[magic]

It's probably capacitance which makes the difference between diodes. Try changing CJO to confirm.

Has it been established that you need those diodes? IMO there are only two issues here:
1. Overvoltage from external circuitry damages the opamp. 10kΩ plus internal protection of most opamps should prevent this to a reasonable degree.
2. Weird output from the opamp damages circuitry outside the TIM module. Is this a concern of any sort?

[aqibi2000]

How have you verified it is faulty?

Inside is most likely a standard SOIC

[LoveLaika]

I haven't physically confirmed whether the diodes are necessary. Like you said, they seem to be for overvoltage protection. As for the second concern, I don't think it necessarily is a problem. The output of the IVC goes into another pre-amplifier which converts it to another voltage (with respect to another reference voltage than the one in the IVC). You can see it below. Output goes to LG6 and the reference voltage of the IVC goes to LG7. In my case, option E is not present when the IVC is present. Conversely, when option E is present, the IVC is not.

From what others have said, if the diodes are used for just circuit protection, then a 1N4148 will work in lieu of the BAV45, despite the horrid simulation results below. It could, like you said, be an issue with the SPICE model. Honestly, it's been so long, I don't exactly remember where I got the BAV45 SPICE model. You can see how I'm simulating it below. Maybe it's just a matter of me simulating it incorrectly. Sending a square wave current source, you can see how it's being converted into a voltage. Protection diodes slow it down a bit, but the conversion is still clear with some diodes while others distort it.

[LoveLaika]

I haven't verified that the IVC is faulty. It's just that according to one of my professors, when removing the connector, the leg snapped off of the case, and epoxy was used to 'glue' the leg back on. Due to being unable to test it, and due to the part being really expensive, they want a replacement. Thus, I'm doing my best to try and build an identical circuit with the information provided. I suppose you may be right, being a standard SOIC, but there's no way without cracking it open, and that's not a risk that they are willing to take.

[magic]

What I say is that a diode with too much capacitance will slow it down.

Regarding protection, I asked if the diodes protect the input side from the TIA. Is there any concern about the signal source being damaged if the TIA applies more than 0.7V to it, despite the 10kΩ series protection? If not, maybe just get rid of the diodes.

[LoveLaika]

The input current is coming from the tip of an STM. As that current goes through the IVC going through that 10k ohm resistor, Ohm's law, I0 has a voltage. Correct me of I'm wrong, but that's the voltage you're talking about at the input signal source? With regards to that, the max input voltage that we can put at the tip is +-10 volts, so i think we're okay.

Going through some other comments and asking around elsewhere, I kind of realized how dumb I was. Below is a simulation of mine, using the ideal op-amp model and the 1N4184 model (comparing it to the BAV45). Someone mentioned a feedback capacitor, and that seems to magically solve that ringing issue I posted in my previous circuits. Here, I thought it was a bad model, but it was probably the parameters itself. Previously, I didn't add in that feedback capacitor because the original schematic didn't show it, but I guess I need it now if we're switching diodes.

Unfortunately, that brings up the issue of how to get a feedback capacitance that small. Lowest I can get is 100 fF. @magic, I really appreciate all the help you've given me, and I apologize for not realizing this sooner, but in your experience, how would one achieve such a low capacitance? (or maybe it might be easier to use a different diode; then again, this is an ideal op-amp, so perhaps things will change when using a real op-amp model)

[LoveLaika]

@KeepItSimpleStupid Thank you very much for your earlier replies. Sorry, I've been revisiting this issue, and taking into account your advice by adding a feedback cap, it's been very helpful. You can see in my posts with ideal opamps how a feedback capacitor helped when I used different diodes. Now, I'm kind of experimenting with that idea, trying various diodes and op-amps in order to see what would be useful. You can see it in my attached simulation below. Compared to an ideal op-amp model, you can see how the addition of diodes and the feedback capacitor affect the output.

Sorry for rambling. I was just excited at the prospect of getting some progress, I wanted to show this off. Thank you very much for your help. If you don't mind me asking, looking at these results, what do you think so far?

[magic]

I have no experience besides building the TIA picoammeter with LMC662 and, more recently, designing a audio bandwidth TIA-like circuit which I haven't even built yet

You can't have more than 50fF feedback capacitance IIRC. I posted about it long ago, it's no rocket science but basic math. From the limited experience I have, I can tell you that you will probably need to connect a bunch of smaller resistors in series just to get their parasitic capacitance under this target. You don't need to shop for 50fF capacitors. Hell, even the opamp will have capacitance between its pins, better use a single rather than a dual for that reason alone.

Instead of throwing feedback capacitance at the oscillations, remove as much of input capacitance as possible to prevent them from occurring. You must find some low capacitance, low leakage diode. Sorry, can't help with that, but 1N4148 will likely fail on both counts, forget it. You can connect a few diodes in series if neither the tip nor the opamp needs protection from voltages lower than a few volts, this will reduce capacitance and leakage.

Maybe omit the diodes if you feel adventurous, but consider if there is a possibility of 15V or whatever appearing at the output node under some fault conditions and finding its way through the feedback resistor to the tip. And whether it's a problem, conidering all the series resistance along the way.

Out of opamps available in LTspice, try LT1169 or the LT179x. Low input capacitance IIRC and low input noise current. You could also run noise analysis, LT includes noise models of their chips. Run AC analysis, run transient analysis with sinewaves.

I have no idea how much noise and GBW you need. GBW helps the opamp hold IN- at zero volts and reduce effects of parasitic capacitance on IN-. It also reduces input impedance seen by the tip. Well, there are some very fast JFET opamps like OPA627. It doesn't help that no one knows what was in the original module.

[LoveLaika]

Thanks for your reply @magic. With the tests I ran at 50 fF, I was working with the ideal op-amp model. Things certainly changed around when I started to use non-ideal op-amp models. You can see that in my other reply to @KeepItSimpleStupid. Using the OPA602 as a start, the feedback capacitance increased to something more realistic at 0.1 pF. Thinking about what you said, I never did account parasitic capacitances that come with resistors. Taking that into account, I may not even need that feedback capacitance depending on the op-amp and diode I choose?



I was working with the 1N4148 to use as a 'control' of sorts to see how to work with it and use that as a jumping off point. That diode is very common, so I figured that working with that will give me an idea of how to move on when working with other diodes. The issue with the BAV45 that I believe was used previously is that it is now obsolete. It had leakage current in the pico-amp range (and capacitance of ~1.3 pF), and I can't find that or any alternative part with that low leakage current in any available/in-stock part on Digikey. The idea was to try and work with easily available parts so I don't have to spend a fortune trying to find some part like the BAV45.

Believe me, I wish I could see what was in the original module, but opening that up and seeing what's inside is out of my hands.