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, several times the price of my 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.
Sapphire
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 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 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.

I'm still undecided at this moment, between buying or making.
So, also 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.

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 all of them out in LTspice to learn about the circuits and see if I could tailor them to my needs.

The 3 Major Typologies

There may be more, but this is what I focused on. Note that 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.


Next is the more traditional Instrumentation Amplifier Design


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

The Gerber files are available, so this design can be duplicated rather easily. Note that the Gerber files on the website 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 Conrad.com.

Here is the above 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


I found this typology 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 (Conrad.com), 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 stay below 1V, we can use attenuation circuits for 10V, 100V and 1000V and hope to keep 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 yet.


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 1000V. 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 and output at the circuit of 1V, 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 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 (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 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, even with the -20dB attenuation. The LT1818/19 however have 10uA, which is a lot higher! This current will cause an error of 90V over the 9M resistor. For me, that error 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 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 good, but the reverse current per diode is 2.5uA, adding 5uA to the error budget for each input channel. This causes a voltage drop over the 9M resistor of another 45V!

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. I think I can manage to solder two individual SMD diodes in place of the BAV99 on Kalle's PCB.

After (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, also based on my little stash of high voltage resistors in the 1+M range.


Common-Mode Rejection Ratio (CMRR)

The whole reason for using a differential amplifier is to measure the voltage  difference between 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 are exactly the same. This challenge is probably the most important reason for the price justification for these commercial probes. The THS4631 lists a CMRR of 80-95dB, so that should be the goal.

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

If you look at the various circuits, 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 must be equal in value, so a small 100-500 Ohm trimmer, here shown with R15 and R16 in the mid-point position, will allow to tweak that. 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 at the output of the amplifier with a fast rise pulse.


Input Protection

I want to add some form of input protection for the expensive op amps, so I'll add a set of 1N4148 diodes to the voltage lines so that 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.

Here is a complete circuit diagram for 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.


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.
For starters,  I will only populate one PCB, the one that I will use the most, the 0-10V version.
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 the 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 the Micsig one, 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...

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 a set of the 499R and 49.9R resistors.

While continuing to learn and play with this, I also did 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.

Well, I 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, 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 put them back to 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 large 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.



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 see this:
Micsig Combo offer
The offer is not valid anymore, but you could get two for the price of one. I almost pulled the trigger...

Maybe, just maybe I'll go for the make & buy option.

"I want it all, and I want it now!" Queen. 
  • One DIY with no attenuation for 1V levels with the highest bandwidth for shunt measurements.
  • One DIY probe with 10x attenuation for logic levels at the highest bandwidth.
  • One DIY probe with 50x or maybe 100x attenuation level for a max of 50V or 100V for AC/DC Power Supply levels with a high bandwidth. 
  • Two Micsig DP10013 probes at 1300V for line level measurements.
The DP10013's are listed as having 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, and with my DIY probes, I can hopefully fill the gap at the lower voltage levels.

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.

Stay tuned for more...




No comments:

Post a Comment