Show by Label

Sunday, October 22, 2017

Differential Amplifier Probe : Make, Buy or Both?

Why (I think) I Need a Differential Probe

After I sold my trusted Fluke 123 ScopeMeter, I lost the ability to connect probes where ever I wanted to, without thinking, or risking damage.

With my new -earth grounded- scope, I need to be extra careful to avoid making shorts by clipping the ground leads to the appropriate spots. Something I need to get used to again.

The answer, of course, is to use a Differential Probe as the front-end to an ordinary, ground or rather, an earth connected scope. As has been reported many times before, these instruments are ranging in price from expensive to outrageously expensive, even to several times the price of my 350MHz scope.

Buying Options

A new offering just came on the market, and that particular probe of 1000V @ 100MHz can be had for about $160.
Micsig Differential Probe
Unfortunately, there are no reviews that I could find yet. The specifications are very good for this price. Too good maybe?

The almost industry standard probe is available from many sources, and is made by one company.
It's about the same price, but only offers 25MHz, the 100MHz version is a lot more expensive.
Professional Differential Probe

Depending on the applications for a probe like this, it's important to list what you really want to do with it. In my case, I occasionally want to look at line level voltages, and for me that means 230V AC at 50Hz. For that 25MHz is plenty. I don't have 3-phase voltages, so 500V is plenty and safe enough. I'm a hobbyist, so official CAT III is nice to have but an overkill if you know what you're doing. (note the word kill)

Other applications I more regularly do is measuring in not ground connected circuits, like across a series shunt in a power supply. In that case, we're talking levels of a few milli-volt to a few volts, but the potential is most likely between 15-50V DC. Other applications are across collector/emitter or source/drain measurements, with the same voltage levels (<50V DC). In those cases, I would like to measure higher frequencies, together with their harmonics, or with a decent pulse/edge representation and in that case, having a bandwidth of 100MHz gives you the headroom that a 25MHz probe just can't give you.

For the majority of my applications, 50V @ 100MHz is plenty, so do I really need to spend $160 for a 1300V safety net, or can I build something myself?

When you look under the hood of these commercial probes, there is not a whole lot there that would justify the price.
Under the Hood
More details
Reverse-Engineered Schematics

DIY Investigation

If you look at the schematics, the value of the parts is not a lot, except for maybe the dual JFET, which can cost about $10-20. So the rest must be labor time in additional manual assembly and adjusting these probes during final test, and of course very healthy profit margins. If you look at the Sapphire 25MHz version probe circuit, apart from the attenuate section, what is standing out are the many R/C filter components and adjustments. If you look at the pictures of the board, there are several parts that look like they were added, tweaked or changed during the testing or calibration. It has all the looks of an untamed tiger to me.

For quite some time, I was on the fence between buying or making.
So, as a matter of interest, I spent quite some time trying to understand what the difficulty is in building a DIY version that will do what I need. Unfortunately, there is not a whole lot of DIY information on the Web, which surprised me a bit.

In essence, what you need is a differential input and a summing amplifier between the Device Under Test (DUT) and the scope. I found three different typologies that were described in various posts when I did my searching. I tried several of them out in LTspice to learn about the circuits and see if I could tailor them to my needs.

Here is a design that has been done for the automotive industry. I don't have the full paper, you need to buy that, but there is some interesting information that can be gathered from the pictures and tables.
Information is here : link
Among the viewable information is a comparison between the various commercial offerings:

The 3 Major Typologies

There may be more, but this is what I focused on. Note that for this topology section, I used one of my typical go-to prototype op amps, the TL072, which has a JFET input, wide supply voltage range and a Unity Gain B/W of 3MHz. This is just to show the concepts.

Simple single OpAmp design:

Very simple, if you don't need a lot of attenuation, because the frequency compensation becomes a bit cumbersome, and it's not so easy to get the required bandwidth. Using only one op amp to do everything has it's price. Here is an example circuit : Here
 The site is in Dutch, so you may have to use Google Translate.

Next is the more traditional Instrumentation Amplifier Design. You can build this using separate op-amps, or use a "real" differential op-amp (also called an instrumentation op-amp) like the AD8421.

Because this seems to be the most logical circuit to use, I spend quite some time trying to understand and to make this work for me. The good news is that it's easy to adjust the gain, by changing R8, the 100K resistor. The not so good news is that there are 6 resistors that need to have the same value (the 499 Ohm ones). Otherwise, the gain, or the CMRR is compromised. I found an application using this typology here : Example
And also here : Here  This one is in Dutch so you may have to use Google Translate. Here is another one: Here
Unfortunately, both projects were not completely finished but have a lot of excellent information.

The Gerber files for the first and third project are available, so these designs can be duplicated rather easily. Note that the Gerber files on the website for the first project are not complete and have errors. I contacted Kalle to see if he is willing to update the information. Kalle used the LT1818 and LT1819 (dual version) for his design, but there are some things you need be aware of when using these op amps. These op amps are relatively inexpensive with 2,53 Euro for the -18 and 5,17 Euro for the -19 version at

Here is the first project as a circuit in LTsim:

As you can see, the simulation does not allow for more than 100MHz, still OK for my use. But this circuit needs some more work. See below.

And finally, Topology 3
This one is really straightforward.

I found this typology on a website here : diff amp probe

As with the previous design, Steven shared his design and Gerber files on OSH Park, so there are PCB's easily available. This is important, because I don't underestimate the layout challenges for 100MHz signals myself. The other thing I like is the utter lack of frequency compensation needed for the THS4631 he selected.
One down side is that this critter is rather expensive at 11,63 Euro (, and you need 3.

Here is the LTsim circuit with the THS4631's.

From the Bode plot, it is immediately apparent that although the op amp is specified for 325MHz when operated in Unity Gain, the summing amplifier action reduces this to about 108MHz @ -3dB. The Bode plot for the outputs of Unity Gain buffers U1 and U2 were indeed about 350MHz @ -3dB.

This simple circuit did not need any frequency compensation at all, which should not be underestimated.
Here is the Step Response with an input of 1Vp-p 50ns pulses with 100ps edges.

Looks great to me. To make this circuit usable, we now need to look at the maximum input and output voltages. The overall probe circuit is designed to have Unity Gain, so what goes in, also comes out at the same level.

Slew Rate
However, here is a hurdle that we need to keep in mind. The Slew Rate (SR) of an op amp determines the maximum voltage swing we can expect at a certain frequency. Normally this is no big deal, but when you're working at the limits of the bandwidth, this "rate of change" becomes an important factor.

The TI datasheet for the THS4631 has this:
High Slew Rate:
- 900 V/us (G=2)
- 1000 V/us (G=5)

There is no unity gain number listed. In any case, what this means is that with a 1V voltage swing (From 0 to 1V) at 100 MHz, we will need a minimum SR of :
     2 x Pi x 1V x 100MHz = 628 V/us

Or, in other words, with the THS4631, we can only go from 0 to 1.4V max. @ 100MHz.

The LT1818/19 has an SR of 2500, much better, but still not enough for 5V logic levels.

To circumvent that limitation, we will need attenuation for the input signals. If the input levels to the op-amps stay below 1V, we can use attenuation circuits for 10V, 100V and 1.000V and still have hope to keep close to the 100MHz bandwidth.

It's unclear how Steven works with his circuit without attenuation, maybe he uses a 10x or 100x scope probe. I have asked him for his comments on this, but I did not get a reply from him at all.

Input Attenuation

For my applications, it makes sense to have a 10V max input level for logic signals, 100V for higher voltages like power supplies etc., and 500V for mains related voltages. I'm going to design that last stage for 1.000V. This makes the math easier when you look at the scope signals, because the attenuation will be 10x (-20dB), 100x (-40dB) and 1.000x (-60dB). This will allow me to have a maximum input of 1Volt and also an and output of the circuit of 1V going to the scope, and that is well below the maximum SR value.

In principle, the attenuation circuit is a combination of a resistor divider for the lower frequencies and a capacitor divider for the higher frequencies. The simple version looks like this:

Before I started to investigate differential probes, I did not yet know the seemingly magic relationship between the above component values. Apparently, for a flat frequency response from DC all the way up to the (in this case) 100MHz bandwidth, the two capacitors have to have the inverse ratio as the two resistors have.  Initially, I was surprised to see several input circuits from very different designs that all came down to this basic circuit. I tried a few variations in LTsim and they all worked. I learned something new again.

This basic circuit can be easily changed for 1.000x or 10x attenuation by changing the resistor values and keeping the capacitor values with the same ratio.
To calculate C3, divide R1 by R2, and multiply that (ratio) result times the value of C2

         C3 = R1 / R2 * C2

In the above circuit, the DUT will see a loading impedance of just over 1M Ohm (1M + 10K). This is the equivalent of a passive 1x oscilloscope probe, which still may be too high of a load on the DUT and could even influence the operation of the DUT, causing measurement errors. The Sapphire probes (the 9001 version) use 4 Meg and 26K dividers, resulting in a 0.65 attenuation factor, and this result gets amplified later on. I would like to keep Unity Gain from input to output, so that limits me to decade numbers to make the math easy.

The higher impedance is more important for me in the 10V and 100V probe versions, due to the circuits I will probe. In this case, going to the equivalent of a 10x scope probe (10Meg impedance) is desired. This higher impedance can be accomplished by using a series resistor of 9Meg together with a 1M resistor, resulting in a 10Meg impedance to the DUT. Alternatively, you could go half way, by using a series resistor of  4 or 5 Meg.

For the 1.000V version, it's not so much the loading of the circuit, but much more the safety aspect that plays an important role. So in this case, you could still use the 9M resistor, but combined with a 10K instead of the 1Meg, resulting in a x1.000 (-60dB) attenuation. The 9Meg resistor MUST be a high voltage version, or otherwise a composition of high voltage resistors in series that create enough of a spark gap and creeping distance between the DUT input and the rest of the probe circuits.

At this moment, and for the simulation phase, I'm using the following values:
For the LT1818:
10x (-20dB)     1M || 12 pF and 111K111  || 108pF
* See Measurement error below

For the THS4631:
10x  (-20dB)     9M || 12 pF and 1M || 108pF

For both:
100x  (-40dB)   9M || 12 pF and 90K909 || 1.188nF
1.000x (-60dB) 9M || 12 pF and 9K009 || 11.988nF

Measurement Errors

Due to the high input resistor value of 9Meg, there will be a measurement error caused by the 1.5nA input bias current of the THS4631 buffer amps. This is acceptable to me, even with the -20dB attenuation factor. The LT1818/19 however have a 10uA bias current, which is a lot higher! With a -60dB attenuation and a 1.000 Volt input, this current will cause an error of 90V over the 9M resistor. For me, that error even with the -20dB attenuation is too large. When that is a concern, you need to lower the resistor values. In many cases however, precision at this voltage level is probably not needed, and loading of the DUT is more important. An interesting dilemma.

Another error source can be caused by the protection diodes. Kalle used BAV99 diodes. Their added capacitance to the input is only 1.5pF each, which is very good, but the reverse current per diode is 2.5uA, adding 5uA to the error budget for each input channel. At a 1.000 Volt at the input, this causes a voltage drop over the 9M resistor of another 45V! Keep those error conditions and causes in mind.

I suggest you use the 1N4148 in the SMD package. Their added capacitance is a little higher at 4pF, but the reverse current is only 25nA resulting in a voltage drop of only 0.2V.

When I have a running version of the amplifier section, I will prototype and decide on the final input resistor values that I will use.

Common-Mode Rejection Ratio (CMRR)

Apart from measuring signals while not connecting one probe connection to earth or ground, is to measure the voltage difference between any two points in a circuit. The added benefit is that any coupled noise that is entering the two measurement leads, get subtracted out, so you can see and measure the pure signal. For our differential probe, we need to take some steps in order to keep the CMRR as high as possible. This means that the resistance and capacitance that are presented at the input of the input buffers and the summing amplifier need to be exactly the same. This challenge is probably the most important reason for the price justification for the commercial probes. The THS4631 lists a CMRR of 80-95dB, so that should be the goal for the overall probe.

To allow for inevitable component tolerances, we need to make the attenuation circuit somewhat adjustable to make both input connections (arms) equal.

If you look at the various circuits in the above examples, they all boil down to an input attenuation section that looks very much like this:

Both the 12pF capacitors can be constructed by putting 4 x 47pF capacitors in series. This will even out the tolerances, and will create a "spark" gap between the high voltage input and the 1V level output of this circuit. Any remainder high frequency adjustment can be made at the summing op amp, to account for any other capacity issues on the PCB, I hope.

The resister divider of both inputs must be equal in value, so a small 100-500 Ohm trimmer, here shown with R15 and R16 as if in the mid-point position, will allow to tweak that. The size of the trimmer will be dictated by the level of matching you can do on the resistors in the first place. The precision is less important, their identical values is. The 108pF section is a composite of a few capacitors in parallel. A capacitor trimmer will allow you to set the precise level, and that can be seen and adjusted at the output of the amplifier with a fast rise pulse.

Input Protection

If I can, I want to add some form of input protection for the expensive op amps, so I'll try to add a set of 1N4148 diodes to the voltage lines so they will clamp the inputs. The standard 1N4148 diode only adds 4pF, which is better than the typical 10-12 pF for a TVS diode. Besides, the 1N4148 is very inexpensive.

Below is the complete circuit diagram with the 10x attenuation (-20dB) using Steve's design. This can also be the base architecture for the x100 and the x1000 versions.

My hope is that I can use the amplifier circuit boards that are available through OSH Park, the Version 2 model, and add the three different front-end attenuate sections to them. Below are pictures from Steve's site:

At this moment, I'm pretty confident that I can make this work.

Reality Check

Now, just for a reality check:
What will the DIY make method cost me? Let's use Steven's design for this.

The 3 PCB's (minimum qty) from OSH Park will cost me $ 3.70 incl. shipping.
3 x THS 4631 will cost me 11,63 a piece, so about 35 Euros without shipping.
The rest of the parts is small change, say 10 Euro incl trimmers and SMA connector and maybe another 10-15 Euro for a case.

That will set me back at least 60 Euro's for one probe, so I can possibly get 3 probes for the price of one Micsig, but I don't get the test leads and adapters with it, nor do I have the means to really test the 1.000x version for the high voltages.

If I go the LT1818/19 way with Kalle's design, the chips are lower cost (only 8 Euro's per board), but due to the loading issues, there could be more at stake with these chips that I have not uncovered yet. The PCB has more real estate, so will be a bit more expensive. All in all, this route will still be less expensive, possibly between 20-25 Euro's less.

If I'm really brave, and consider making my own PCB, I will combine the two circuits. I will then use the THS 4631 for the input buffers, and the LT1819 for the summing amplifier. I tested that combination with LTsim and that works fine.

Hmmm, I need to think a bit more about the make or buy decision before I pull the trigger either way...

Update 31-oct-17:
I pulled the trigger on the THS4631 version, and ordered the PCB's, the chips (I found a source with 10 of them for about 43 Euros) and ordered enough of the 499R and 49.9R resistors to find some matched sets.

CMRR Simulation
 While continuing to learn and play with this project, I also learned how to do a CMRR simulation.

I'm not an expert, but this looks pretty good to me. A possible caveat is that LTspice may not do CMR simulations very well.

I also found a couple of hints and tricks to do a better analysis by using a Monte Carlo model for the most critical parts that have the greatest influence on the CMR. Obviously, they are the resistors and trimming capacitors for the attenuation input, and then the two resistors for the summing amp. The other components did not make a sizeable difference, so I left them at their previous fixed values. I used 1% for the attenuation resistors, 5% for the 12pF, 20% for the trimmer caps, and 1% for the two 499Ohm resistors for the summing amp.

These two last resistors largely define the CMR for the op-amp stage. I will need to carefully select them for a matched set out of the batch that I ordered.

Still looks pretty good to me with an average of about 84dB, and a worst case of 72dB. My goal was to get close to the 80-95dB set by the op-amps.

It will take a few weeks for the parts to arrive, but when I have the boards and populated one, I will start to work on the attenuation values.

Update 2-Nov-2017:
And then..... you get an email from Micsig with a special offer; two probes for the price of one!:
Micsig Combo offer
The offer is not valid anymore, but at the time, I almost pulled the trigger...
The current prices (aug 2019) for the Micsig DP10013 are now 170 Euros (incl. VAT).

The DP10013's are listed as having a spec of 1.300V and 100MHz, but that seems highly improbable with their front-end probing leads. I don't really care, because when I probe at line levels, a minimum of 25MHz is most likely enough, and the safety aspect is much more important for me. The DP10013 50x and 500x attenuation levels are more tailored to higher voltages and line level measurements.

In the meantime, the parts arrived and I completed the build of the three boards. A quick initial test showed that they all work fine. I need to finish a few other projects before I start to work on the attenuation circuits and do more measurements.

Update august 2019:
After I started this post and project, I left it alone for just almost two years. There were other projects that were more importent, and I did not have the tools I wanted/needed to really finish the probes. As an example, I did not have a fast rise pulse or a function generator that would go beyond 100MHz. Since then, I finished my project that would give me the fast rise pulse, so I can finally test and adjust the high frequency responses. I also moved away from Eagle and learned to work with Diptrace, including producing PCB's. And then, I also purchased the equipment to handle SMD parts. All these elements and steps were required to continue with this project.

I'm definitely NOT buying!
Interestingly, during this whole period, I never had the urging need to use a differential probe. This made me realize that buying a Micsig kit is not justified for my typical applications.

I'm making!
I have just ordered the parts for the attenuation sections, so when I have them, I can start to work on the PCB's. In the meantime I will prototype the front-ends and start some measurements.

Update Sept 2019
Believe it or not, but I have finally started again on this project.
Now that I have some better equipment, I can start to profile the amplifier boards.
At first I was a little disappointed when I saw the first results of the fast edge pulse response.
I made sure to stay below 1Vp-p to avoid slew-rate issues, but still...
Here is the screen shot:

Don't you love that fast rise pulse from the Tektronix PG506? I do!

To fix the hf response, I kludged a small 0-10pF variable capacitor with tiny strands to the very tiny pads across the output amplifier feed-back resistor, and tuned it for the optimum pulse response. Things started to look a lot better already. I measured the trim capacitor to be about 3pF, so that is the value that I soldered in place. Steve used a 1pF value on his board, but the Texas Instruments datasheet lists 5.2pF for this configuration. Just for reference. 

Here is the result of that tweak:

Could be a bit better, maybe I should try another value, but I did not want to fiddle too much with this at the moment, in fear of damaging the tiny pads on the pcb. I'll try a few other values on one of the other amplifiers boards. Update: I tried various other values, also with the other two boards but I'm not getting a much improved situation. I'm using 3pF for now.

You probably notice the rise time difference and phase shift. The fast rise pulse response of the amplifier is 3.3nS. Using the Bandwidth formula with the 0.4 factor, this should theoretically be 133MHz. Not bad at all.
To reiterate what I mentioned earlier, I can't verify the bandwidth with a sine-wave, because my FY6600 function generator is the 30MHz version.

Next step is to build a prototype 10x (-20 dB) attenuation board and have a look at what that does.

Below is my first attempt, it follows the schematic diagram of the -20dB version above, but without the protection diodes:

I have used 3 x 3Meg resistors in series to create a 9M resistor. Parallel to that string is a set of capacitors to get to the required 12pF. This is repeated for each input. There are 2 x 47Pf capacitors in parallel with the 40 pF trimmers. The terminating resistors are 1Meg and they are tied to ground with a 10K trimmer. I used 10K because the resistor values of the 9M and 1M are less than perfect, so needed much more tuning than the 100Ohm trimmer I put in the diagram above.

The -20dB attenuation is within a few percent at low frequencies, as can be expected. Unfortunately, with higher frequencies (above 500KHz)  I am getting oscillations.  I need to rethink the way I'm building this front-end and maybe go to a pcb layout already, something I wanted to avoid just yet. I don't know enough and have zero real experience to come up with a good pcb layout and frequently turning boards is what I want to avoid.

I have designed a pcb for the front-end, and sent it out to production. Here are the pictures of the layout. (I'm using DipTrace)

I put in a few extra places for components so I can fool around with this a bit. This is a test version that will allow me to setup different attenuation factors.

In the meantime, my long awaited nanoVNA (Vector Network Analyzer) tool arrived, and after some playing around with it, I decided to give it something to chew on. I created a calibration of the unit using the connectors and cables I was going to use, and then connected the amplifier.

The amplifier input is connected to CH0 (stimulus) and the output to CH1 (response) of the VNA. I set the frequency span to start from the minimum at 50KHz to 250MHz. Here is a picture of that setup and the result:

The two leads going to the input of the amplifier are supposed to mimic the flying leads I'm going to use later with mini grabbers to the DUT, at least that is my hope. I first calibrated the nanoVNA with this cable attached without the amplifier and used the typical open-short-load (50 Ohm) at the end of the cable. The output of the amplifier is 50 Ohm, so that should match with the input.

(note that in the lower left hand corner of the sheet, I scribbled notes while trying to use the NanoVNA to measure the bandwidth of my scope. It passes the 300MHz easily. One point to note is that the NanoVNA uses tricks to get beyond 300MHz, and to compensate, it increases the output volume, making it more complicated to find the real -3dB cutoff point for the scope)

Here is a screenshot of the PC program that talks to the NanoVNA, and allows me to use my normal glasses. The screen is very small, and the type fonts extremely tiny, not helping with my deteriorating eyesight.

I got this display after fiddling a bit with the curve of the input lead. This result looks a lot cleaner. What I think we can see here is that the output of the amplifier has a small 6dB rise at around 60MHz, and then stays just about flat until the -3dB point at about 145 MHz.
Not bad at all I think! Now I need to find a way to see if I can get rid of the 60 MHz issue.

Just when I was about to disconnect everything and call it a day, I noticed that the NanoVNA was still working and collecting data, even though I already pulled the batteries from the amplifier. I noticed that without power, there is the same hump at 60 MHz as we saw on the powered unit. No idea what I'm seeing here...yet

I have the pcb's back from manufacturing, but they are as yet untouched.
To be able to finish the attenuation and frequency compensation, I need to learn much more about using my new NanoVNA, and had to order several SMA connectors and cables for that new tool.

In the meantime, I have a very interesting but for me very difficult project (GPSDO) that I have been working on for several months now. It eats up every bit of time I have learning, tweaking, learning some more, tweaking, ....

Stay tuned for more, I will finish this project, just don't hold your breath.


  1. Thank You for the article - it's a great read.
    Do You plan on publishing Your PCB by any chance?

  2. Yes, I will publish everything.
    I'm still waiting for some parts (slow boat from China), but it's on the top of my list of active projects now.

  3. Great work. What are the advantages and drawbacks of Topology 2 and Topology 3?

  4. @ alterfield.
    I was hoping that would be clear from my post. Drawback from topology 2 is the difficulty in keeping the CMMR low, because many parts need to be matched. That is a welcome plus for topology 3. Frequency compensation for topology 2 is more difficult to obtain than with topology 3.

    1. Thanks for your reply. The frequency compensation for topology 2 is more difficult because there are 3 capacitors to adjust, two of which are the capacitors connected in parallel with the feedback resistors of U1 and U2, respectively, and the other one is connected in parallel with the feedback resisitor of the output stage. For topology 3, only the last one has to be adjusted for frequency compensation. Am I correct?
      Also, I wonder if there will be a DC bias at the output when the input probes are shorted. Some differential probes on the market have a potentiometer on it, which can be tuned to zero the DC bias at the output.

  5. @alterfield.
    You are spot on with the major difference between T2 and T3.
    I have two working diff amps and both are not showing a significant enough offset. However, I did't save the results because I have not finished the front-end, nor the frequency compensation fully, which will dominate the error sources. It will take some time before I revisit this project because there are so many others I'm working on...
    Besides, I do not have a pressing need for the diff probe at the moment.