High Voltage Differential probe design for review - Page 1
Forum section: electronics / projects

author: cjk2
author_rank: Contributor
timestamp: January 20, 2015, 04:03:22 am
content: Here is a design for a 100:1 HV probe up for review. I intend to make this on a simple 2 layer PCB and put it in an aluminum box. Power will be a 15V walwart or bench supply.Perhaps someone that has used a rail splitter before can comment on any problems this design has?I may change to a 200:1 ratio or lower the HV divider impedance if I encounter problems with high frequency response.C7 and C15 are to be used if more capacitance is needed to compensate the probe, possibly due to needing to make all the 1pF caps bigger for some reason.Anyone care to give me a design review?

author: diegosfb
author_rank: Contributor
timestamp: January 20, 2015, 02:31:01 pm
content: Looks very goodRemember it is recommended to have small ceramic caps between the power rails of each opamp to minimize the noise.Let us know how it goes once it is constructed.Best Regards,

author: Marco
author_rank: Super Contributor
timestamp: January 20, 2015, 03:54:08 pm
content: Why make a instrumentation amplifier out of discrete opamps?Have you seen theElektor design? There I can see some reason for the discrete opamps (it also uses a trick to get better CMRR you might want to crib if you stick with it).

author: tggzzz
author_rank: Super Contributor
timestamp: January 20, 2015, 04:17:30 pm
content: It is probably worth running a spice model of the passive components between the instrumentation amp and the probes - making sure you add in some plausible values for parasitic inductance and capacitance. See the component datasheets and PCB design tutorials for suitable values.If you are dealing with high voltages, the protection afforded by having an aluminium case is dependent on the quality the way it is earthed. In a non-ideal world that could be compromised in several different ways. You may like to consider going part way towrds double insulation, by having an insulating plastic box with the metal box inside it.

author: free_electron
author_rank: Super Contributor
timestamp: January 20, 2015, 05:35:45 pm
content: this is not a differential probe as it has no common mode rejection ! the coupling between the first two opamps is missing ...

author: macboy
author_rank: Super Contributor
timestamp: January 20, 2015, 07:01:21 pm
content: Quote from: free_electron on January 20, 2015, 05:35:45 pmYou don't need coupling between the first two op-amps for common mode rejection. In a 'typical' differential instrumentation amplifier, where the first stage op-amps have gain, the coupling between the two first-stage amps ensures unity gain for common mode signals, but programmed gain for other signals. So you aren't really rejecting common mode signals in the first stage so much as simply not amplifying them. Then the following differential amp takes care of rejecting (most of) what is lest of the common mode. In this case, the first stage is unity gain, so no benefit is to be had from coupling the feedback together.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: January 20, 2015, 08:16:58 pm
content: Looks good, but I'd worry about "hook" (slight rise/droop at time constants other than the dominant compensation TC). Curious how good the CMRR will be at higher frequencies.I made a 1000:1 sensor with this sort of design; I used 4.7pF capacitors in the divider chain (I think with the same number of resistors, too), which of course would require a whopping 1nF to compensate, so I didn't compensate it by variable capacitance, I did it by variable resistance. This varies DC instead of AC gain, allowing compensation; a second trimmer sets DC+AC total gain, allowing calibration as well.When you do the layout, mind to keep copper (including ground plane) well away from the dividers! This also serves as isolation/creepage/clearance (since 100x at this voltage range is going to be, what, CAT II range I suppose?). The rest of the circuit should have ground plane, stitched top and bottom if it's two layer.Tim

author: cjk2
author_rank: Contributor
timestamp: January 21, 2015, 12:51:54 am
content: "Why make a instrumentation amplifier out of discrete opamps?"Can you find one that has bandwidth out to 50MHz or so? I would love to improve the design but I have not found any."Have you seen the Elektor design?"I had not until you mentioned it. This is an interesting design but much slower."You don't need coupling between the first two op-amps for common mode rejection."Right, this is what I though and simulation has confirmed.Attached are some simulation results as well as my revised design.CMRR is 28dB worst case and much better for lower frequencies. I wonder if sticking a common mode choke (ferrite core) on both probe leads would help improve CMRR.I will have to terminate on the scope end in 50 Ohms I suspect and suffer the 6dB loss.

author: Mechatrommer
author_rank: Super Contributor
timestamp: January 21, 2015, 01:41:37 am
content: Quote from: macboy on January 20, 2015, 07:01:21 pmread AoE 2nd Ed page 421-426... these sharp people suggesting it as the last improvement man can make for reasons (experience maybe?) wanna reinvent the wheel? go ahead we have no objection.1) you probably wont need 5 gangs of 1M+1pF in each input. maybe only 2 gangs of 2.5M+?pF2) dont put ground plane at the bottom of input voltage divider. that was a "reinventing the wheel" mistake i made during my ver1 pcb design. i figured out later... everybody are not doing it. need to prove that thesis in the ver2 pcb later in the unknown future.3) what bandwidth are you aiming? anything below 10MHz is pretty much practical for hobby build in practical time frame with practical CMRR requirement imho. i suggest make a literature study before wasting money.ltspice CMRR 1.png (17.58 kB, 1473x591 - viewed 5 times.if only ltspice is true (100dB? CMRR), i want one! you'll smoke the hell out most of hi-volt diff probe out there including agilent 1141a+2145 100X setup (only 52dB). but alas imho this is the arena where many spices failed... ymmv. note: its not the spices sw that failed, its the components model you are using that are. and please do keep in mind even a short copper trace is a "component".

author: cjk2
author_rank: Contributor
timestamp: January 21, 2015, 04:00:48 am
content: Here is a draft of my layout. I am aiming for 50MHz but will not be upset if I get 10MHz only.

author: Richard Head
author_rank: Frequent Contributor
timestamp: January 21, 2015, 09:29:26 am
content: In the interest of better CMRR would it not be better to increase the gain of the differential amp stage? As it is there is no difference between the common mode and differential mode gain.

author: Dago
author_rank: Frequent Contributor
timestamp: January 21, 2015, 10:04:56 am
content: I designed a high-voltage (designed for 500 Vrms) differential probe last year:http://www.dgkelectronics.com/storage/electronics/differential_probe/differential_probe.pdfhttp://www.dgkelectronics.com/storage/electronics/differential_probe/layout_screenshot.pngI built one prototype but I have quite a bit of DC offset on the output due to the opamp input current. When I get around to it I'm going to swap the voltage divider resistor values to smaller ones.I got it tuned up pretty well in the simulation (-3 dB bandwidth of ~150 MHz, I'd be very happy if it actually did 50):http://www.dgkelectronics.com/storage/electronics/differential_probe/lt1818_tuned.pngFinding a suitable op-amp was very challenging. Even the LT1819/1818 is not very optimal because of the high input current (I haven't managed to find a better one though).I haven't gotten around to measuring the CMRR (need to fix the offset issue first). It seems that the opamp SPICE models I used are somehow simplified in terms of modeling the CMRR and the simulation does not seem to change much even if I swap the opamps to some totally different ones. Need to look in to that.

author: Marco
author_rank: Super Contributor
timestamp: January 21, 2015, 07:53:43 pm
content: Quote from: cjk2 on January 21, 2015, 12:51:54 amAD8129/AD8130?

author: cjk2
author_rank: Contributor
timestamp: January 22, 2015, 02:39:31 am
content: Dago:Thanks for sharing your design. I changed to the LT1819 after looking at its specs. It seems better than the opamp I had selected. They are pin compatible so I may well build both and see which one performs best.Marco:The AD8130 looked interesting at first but does not have much better CMRR than my solution appears to. I think this part could be used and may be superior in some regards but may have trouble driving 100 ohms as I will need here. The AD8130 plus a power driver could work well though and I may try it at some later time.Attached is my latest schematic and the board I am about to send off.

author: Jay_Diddy_B
author_rank: Super Contributor
timestamp: January 23, 2015, 07:21:54 am
content: Hi,I would suggest replacing the 1pF capacitors that you have in parallel with the input resistors with 20pF capacitors. You then have to make a similar adjustment to the capacitor at the bottom of the divider.If you use 1pF capacitors I believe that you will have difficulty getting a flat frequency response because of stray capacitance. You can add some stray capacitance to your LTspice model like this:I just added some 0.1pF stray capacitance, I am not sure what the value will be, but it does not take very much.The Tektronix P5205A has 5M Ohm // with 4pF per side as shown here:http://www.tek.com/datasheet/differential-probe-high-voltage/tmdp0200-thdp0200-thdp0100-p5200a-p5202a-p5205a-p5210aThere are some pictures of the P5205A in this thread:https://www.eevblog.com/forum/testgear/tek-p5205-hv-differeantial-probe-teardown-btw-what-are-the-red-and-brown-wires/If I look carefully at the picture, it looks like they have 2 x2.2pf in series in each side, this means that the input capacitance is lower than the spec, or there is some other capacitance somewhere else.The results from the LTspice model are:I have attached a zipfile with the model.Regards,Jay_Diddy_B

author: tggzzz
author_rank: Super Contributor
timestamp: January 23, 2015, 09:50:10 am
content: Quote from: cjk2 on January 22, 2015, 02:39:31 amHave you done anything to determine the major contributors to CMRR?It might be worth doing a monte-carlo analysis on the components in the voltage divider, especially using realistic tolerances for the resistors and capacitors when placed on a slightly grubby circuit board. My gut feel, without analysis, is those effects will dominate the opamp's non-idealities.

author: Jay_Diddy_B
author_rank: Super Contributor
timestamp: January 23, 2015, 04:20:12 pm
content: Hi group,Here is a Monte Carlo model for the divider. I assumed that the capacitor in the divider have 5% tolerance and the stray capacitance is 20%. I have set these using parameters so they are easy to change.Here is the model:The result for 1pF capacitors:And for 20pF capacitors:I have attached the LTspice model so that you can play with the parameters.Regards,Jay_Diddy_B

author: edavid
author_rank: Super Contributor
timestamp: January 23, 2015, 04:38:51 pm
content: How do you plan to implement gain, offset, and CMRR trim? (DC and AC for gain and CMRR)

author: cjk2
author_rank: Contributor
timestamp: January 24, 2015, 01:50:54 am
content: Jay:Thanks for your work in simulating the input stage and pointing out the problems with parasitics. I have revised my design to take the effects you discovered into account.edavid: You asked "How do you plan to implement gain, offset, and CMRR trim? (DC and AC for gain and CMRR)"Gain: You get what you get with 0.1% resistors and whatever offset errors and input currents the opamps have. I will be happy if i get to 2% or less gain error but I will deal with whatever I end up with. The terminator on the end of the 50 ohm cable (if I use one) will introduce error anyway (1-5%?).Offset: You get what you get. I can't imagine there would be too much offset error but I have certainly been wrong before. I am not worried about an offset that is a few percent of full scale only. If it is 20% of full scale then I will probably redesign the board with trimmers or choose different opamps. Where would the offset come from anyway? The two input amps will have somewhat close bias currents I suspect so they should not generate much differential offset. The difference amp uses lowish impedance feedback parts so the input current there won't matter much. The only other source of error I can think of is then voltage offset error of the amps which for my parts is about 1mV which will translate to 500mV of input referenced offset or like 0.1% of full scale offset error. Am I missing some other effect that will cause more offset?CMRR: At DC you get what you get with 0.1% resistors. For AC the CMRR is tuned with the trimmer caps on the input stage. The CMRR will get worse as frequency goes up so it makes sense to worry more about that than some small low frequency common mode leakage.

author: Jay_Diddy_B
author_rank: Super Contributor
timestamp: January 24, 2015, 07:52:51 am
content: Hi group,Here is some more Monte Carlo analysis of the complete circuit.Normal Mode GainIn the first model I have configured the circuit to measure the normal mode (Differential) gain:The results show a -3dB point at 100MHzCommon Mode GainIn the second model I have moved the source so that we can measure common mode gain:Here are the results of an ac sweep:And the transient response, the common mode input is a 500V step:Gate Drive ExampleIn this model I have two inputs, I have a 10V p-p input combined with a 100V p-p common mode signal This is would be typical of looking at a gate drive signal on a high side MOSFET switching at 50 kHz.You can see the wide range of results from this test.I have attached the LTspice models in a zipfile.Regards,Jay_Diddy_B

author: tggzzz
author_rank: Super Contributor
timestamp: January 24, 2015, 10:09:19 am
content: You may find some points in this article relevant, since it is the experiences building a homebrew "1GHz differential active probe"https://xellers.wordpress.com/2014/09/28/diy-active-differential-probe-characterization-round-2/

author: Jay_Diddy_B
author_rank: Super Contributor
timestamp: January 26, 2015, 04:55:24 am
content: Hi Group,I spent a little time in the lab with two commercial H.V. Differential probes. One is a SI-9000A, this is made by Saphire Instruments and is available re-branded from a number of sources. The other is a Tektronix p5200. Both are 50x/500x probes. All these measurements were made in the 500x setting. The measurements were taken with a 1GHz TDS784a. With both these probes the scope is used in the 1M Ohm mode.The 100V signal was made by a Tektronix CG5001 scope calibration generator. The unit was used in the 'EDGE' mode. Risetime is less than 100ns, Abberations less than 2%.In the all the picture the purple trace is the signal measured with a Tek P6139A 500 MHz passive probe.SI-9000ADifferential ModeCommon Mode - Both leads connected to the signalTek P5200Differential ModeCommon Mode - Both leads connected to the signalHere is the specifications of the Tektronix probe:Regards,Jay_Diddy_B

author: Jay_Diddy_B
author_rank: Super Contributor
timestamp: February 03, 2015, 12:12:19 am
content: Hi,I did a few measurements on these probes with a HP3577A Vector Network Analyzer.SI-9000AThis is the differential mode gain, a x500 probe should measure -54 dBThe common mode gain is measured by putting the same signal on both leads. The lower the gain is better. It is a measure of the probes ability to reject common mode signals.Tektronix P5200Differential GainCommon Mode GainYou can see that neither of these probes has particularly spectacular performance.Regards,Jay_Diddy_B

author: Circlotron
author_rank: Super Contributor
timestamp: February 03, 2015, 02:00:54 am
content: In the circuit in the first post, C6 will see twice the slew rate than C14 and they are both the same value. What's more, the signal that gets filtered by C14 also gets filtered by C6 but not vice versa. Will this not cause problems at HF?

author: Jay_Diddy_B
author_rank: Super Contributor
timestamp: February 03, 2015, 05:20:58 pm
content: Quote from: Circlotron on February 03, 2015, 02:00:54 amI can build a model of that part of the OP's circuit and measure the gains. I can measure gain from the inverting input, non-inverting and the common mode gain.The amplitude response from the inverting and non-inverting inputs is the same. There is (a desirable) difference in the phase response.The common mode gain (rejection) is good at low frequencies but is reduced at higher frequencies. This comes from the LT1807.Regards,Jay_Diddy_B

author: Jay_Diddy_B
author_rank: Super Contributor
timestamp: February 04, 2015, 04:43:28 am
content: Hi group,I took my Saphire SI 9000 probe apart for some photographs.When you open the case you find two screened boxes.Under the first box there is a power section. This is used to generate +/- voltage from the 6v battery:Under the other box is the input section and amplifier:Regards,Jay_Diddy_B

author: Jay_Diddy_B
author_rank: Super Contributor
timestamp: February 04, 2015, 04:55:18 am
content: Hi,I was intrigued by the poor performance of these probes at high frequencies. So I took a closer look.I measured the response using an RF signal generator and an oscilloscope.First the gain at 1MHz:This is correct it is showing a 500x reduction in signal amplitude.At 44 MHz I found a resonance:The gain is much higher than it should be, 23.96mV out with 320mV input. That is divide by 13.3 instead of divide by 500.I noticed that gain was sensitive to the arrangement of the leads.A quick LTspice model shows that the 7pF capacitance of the probes is resonating with a few uH of inductance.I am sure that this could be engineered better to dampen this resonance.Regards,Jay_Diddy_B

author: tautech
author_rank: Super Contributor
timestamp: February 04, 2015, 04:55:46 am
content: Quote from: Jay_Diddy_B on February 04, 2015, 04:43:28 amScrubbed IC's

author: Jay_Diddy_B
author_rank: Super Contributor
timestamp: February 04, 2015, 05:03:29 am
content: Quote from: tautech on February 04, 2015, 04:55:46 amI don't know why they bother.It has a Harris logo, it is DIP, it is a high speed multiple op-amps that has been around for 10-15 years so that should narrow it down to a handful of parts.Jay_Diddy_B

author: T3sl4co1l
author_rank: Super Contributor
timestamp: February 04, 2015, 12:55:49 pm
content: Try ~500 ohms in series with the "probe" lead.Note that, even if the differential and common mode sensing is constructed with zero capacitance, you still have the loading effect of the freaking meter (give or take) of wire, which itself becomes resonant at 75MHz or so, with a characteristic impedance of maybe 100-300 ohms differential mode, and 50-600 ohms common mode, depending on how the cables are routed together and what they're laying on.Tim

author: Jay_Diddy_B
author_rank: Super Contributor
timestamp: February 04, 2015, 01:35:54 pm
content: Tim,I had similar thoughts myself. The 500 Ohm series resistor will damp the resonance.A similar result is predicted by SPICE:I found the calibration procedure for the SI9000 probe here:http://www.sapphire.com.tw/si9001cp.htmI hope these measurements help the original poster with their design.Regards,Jay_Diddy_B

author: cjk2
author_rank: Contributor
timestamp: February 07, 2015, 08:13:44 pm
content: I want to thank you all for your hard work and investigation on this project. I have ordered my boards and parts today. Hopefully some time in the next month I will be able to build and test this thing!

author: janaf
author_rank: Frequent Contributor
timestamp: February 09, 2015, 03:17:42 pm
content: Just popping in on this thread, you might want to look at fully differential op-amps for the first stage, like THS4521 / THS4541. TI have a bunch of differentials in the portfolio.

author: AdShea
author_rank: Contributor
timestamp: February 13, 2015, 03:18:29 am
content: Problem with most those fully differential amps (TI or others) is that the input impedance is pretty low (100s of ohms) and the circuit topologies needed are low input impedance which screws with all the work in making a nice input attenuator.For reference, the P5200 used a MAX436 to do the differential to single-ended conversion (and a bit of gain) but those are long gone.

author: janaf
author_rank: Frequent Contributor
timestamp: February 13, 2015, 10:18:20 am
content: You are right.I looked up the datasheet; not hundreds but around 100K; 72K for the THS452X, 110K for THS4541Quote from: AdShea on February 13, 2015, 03:18:29 am

author: AdShea
author_rank: Contributor
timestamp: February 13, 2015, 05:47:19 pm
content: Yeah, I was looking at some really fast video reciever ones that had ~700 ohm differential input impedance. Still have to wire them up in a configuration that has even less input impedance (similar to inverting opamp circuit) if you want to get good noise performance.

author: Mechatrommer
author_rank: Super Contributor
timestamp: February 15, 2015, 04:34:21 am
content: Quote from: janaf on February 13, 2015, 10:18:20 amwrong opamp for the job? maybe LMH6503...

author: AdShea
author_rank: Contributor
timestamp: February 17, 2015, 07:21:10 pm
content: Better, though the bias current might be an issue (11uA typical) also the output-referred offset voltages are in the ~100mV range and change with gain setting and common mode voltage. It's also a bit on the slow side for aping the P5200, but getting closer...I'm almost thinking that transconductance amp-based frontends are the way to go though.

author: dazz1
author_rank: Frequent Contributor
timestamp: November 14, 2024, 06:29:51 am
content: HiSo the last post on this topic was about 10 years ago. Was there an end to this story?Is there a topic that covers a more modern HV probe?

author: timeandfrequency
author_rank: Frequent Contributor
timestamp: November 14, 2024, 02:17:32 pm
content: Quote from: tautech on February 04, 2015, 04:55:46 am'Switching controller' DIL-8 used in the PS section is an NE555 running in astable modus.