Precision Calibratior Project (Voltage and Current) - Work in progress - Page 1
Forum section: electronics / projects

author: Cpuch22
author_rank: Contributor
timestamp: July 06, 2025, 06:28:50 pm
content: Hello,Recently I got the itch to work on another electronics design project, as I haven't done one in a bit. I have always liked designing custom circuit boards and wanted to design something complex. Historically I have always used Eagle for my board designs but since that is going the way of the dodo I wanted to design it in KiCad instead. I have used KiCad before but wanted something more involved to try. This will help knock the rust off my design skills, and help me learn the KiCad interface a bit better.I have always thought it would be a fun project to try to design a voltage and current calibration device with precision components. I don't really have a use for one, but despite this, I think it would be fun project, and be a good learning experience. This post/thread is what I have come up with so far. I started on this over the long holiday weekend we just had, and think that I have made some good progress. I would love feedback from anyone who wants to give it.Here were my design goals:--Precision, Programmable, Voltage output between +/-10V with 10 uV resolution - Will use a 20-bit DAC for this--Precision Programmable current output between 0-1A with 1 uA resolution - Will use the same 20-bit DAC--Temperature controlled for better long term stability - Integrated heater which is controlled by the microcontroller to maintain a constant temperature in the enclosure.--User interface with a screen and controls - I have done lots of microcontroller projects but have never made one with a screen before. Programming is my weakest area, so I am sticking with an Atmel chip so I can use the Arduino IDE.--Good mechanical design in a professional looking enclosure that I can keep on my bench.--Small form factor. I like designing with SMD components.--Dual power inputs for battery or wall powered operation - the idea is you could leave this on all the time for better reference voltage stability, and then plug in a USB power bank if you need to transport it and it would remain powered the whole time.So far the project consists of a front panel PCB to hold the buttons/screen and other UI related components, a main PCB which contains the rest of the circuitry, and then an enclosure to house it all in. I have the design of the front panel PCB mostly complete (schematic and layout). The main PCB I have the schematic mostly complete and have started on the layout. The mechanical CAD I am working on as well in parallel with the board design.Attached are the 2 schematics and some renderings of the enclosure.Cheers!

author: dmendesf
author_rank: Frequent Contributor
timestamp: July 06, 2025, 07:17:18 pm
content: Great project! Keep us posted!

author: Cpuch22
author_rank: Contributor
timestamp: July 20, 2025, 05:52:44 am
content: I've made some good progress on the design of this project recently. The schematic has gotten more refinements/corrections, and and I'm getting close to being done with the main control board layout. I also also have most of the mechanical/CAD design work done too. The main control board will use a 4 layer stackup (SIG, GND, GND SIG), and the display board will be a simple 2 layer design. The front and rear panels will also be 2 layer PCBs since they are cheap and can be easily customized with cutouts and graphics. The enclosure is a Hammond: 1455Q1601 (160m x 125mm x 52mm).Attached are the updated schematics and some renders of the design. If anyone has and suggestions or sees any flaws I would love to hear your feedback. I hope to be ordering parts and boards soon, and it is much easier to correct errors at this stage of the game than after its already built.

author: derZockerMP
author_rank: Regular Contributor
timestamp: July 20, 2025, 01:15:00 pm
content: Hello, just found your nice project. I looked a bit into the schematic and stumbled upon a few things that seem a bit optimistic.First, the output and reference input of the DAC1220 need some guarding around the input pins and capacitors. Also, some high-quality film caps should be used.Second, there is not much headroom to get the full 10V output. All components have small tolerances, and this can add up to not fully reaching the full 10V. Also, the lower end (0V) could be a problem. Normally, DACs have much worse non-linearity in the upper and lower code range, so there could be an error there too. Better to make some headroom in the non-inverting amplifier and calibrate it in the software.Don’t know exactly if the large filter by U6 and U5 is necessary, and they can also load the high impedance (around a few kiloohms) DAC output. For the relays, better use bistable relays to reduce thermal EMV in the relay contacts by heating up with the relay coil.The output TVS diodes should be low leakage ones, to reduce current errors (could be irrelevant because you only have a 1A range).The last point is the current shunt. Self-heating is a big problem here, use low tempco ones. Absolute tolerance is not that critical. Please look at the company Isabellenhütte. They produce nice resistors for such a purpose. You can also consider going to a 100mOhm shunt so the power dissipation—and thus self-heating—decreases. The additional error due to the times-10 amplification of the sense voltage should be lower.In the power supply region, be careful about common-mode noise!Overall, nice design, and the first prototype will give you some indication of where you have to work on.The last thing I didn’t understand: what exactly do you want to heat? The full enclosure or only the critical components?Best RegardsStefan

author: Cpuch22
author_rank: Contributor
timestamp: July 20, 2025, 03:51:35 pm
content: Hi Stefan,Thanks so much for your feedback! I really appreciate it! I will try to follow up with some feedback based on your suggestions.For the guarding of the sensitive components on the DAC I have the VREF signal routed as a guard trace as the recommended in the datasheet. See image below. The capacitors that I have selected are C0G dielectric ceramics. I use C0G for any capacitor that is in the analog signal path. For bypass caps I use X7R. It was my understanding that film and and C0G ceramics are comparable for use in analog circuity. Do you recommend otherwise?Regarding the headroom on the voltage output stage. I had a similar thought this morning and increased the gain on the non inverting output similar to what you suggested. See image below. Gain is now 2.1, which gives 0.5V additional headroom. This should be enough to allow for the full 10V output after calibration.I agree about the filters, potentially causing an issue, with the DAC. I initially selected lower resistance valves to reduce noise, however I do see now that that could potentially load the DAC too much. I could increase the 2 resistors in the filter by a factor of 10x 1.2k -> 12k and 22k -> 220k this would decrease the load on the DAC and would also lower the cutoff frequency from 1000 Hz to 100 Hz both good things potentially. Another option would be to forgo the filter entirely. Worst case I could not install the filer capacitors and install 0 Ohm resistors, which would turn the circuit into a buffer.Regarding the Relays I had not considered the bistable/latching type. I will look into those. With that being said heating might not be a bad thing. The heater circuit in the project is intended to keep the internal temperature of the enclosure elevated and constant. I was going to target around 50 C for a setpoint. There is a thermistor located right next to the DAC and VREF that will provide feedback to the temperature control circuit. There are power "heater" resistors scattered around the analog section of the board, with the majority of them located near the DAC/VREF. See attached image. My thought was that with this approach, along with some insulation, that I would be able to maintain a stable temperature for all the components inside.For the 10x10Ohm parallel current sense resistors I selected: SEI Stackpole RNCF1206AKT10R0, which are 1206 size, 1/4W, 0.05%, and 10 ppm tolerance. The max power dissipation at 1A would be 1W = 0.1W per resistor. I was hoping that this might be good enough but I can look into lower tempco/lower resistance shunts. See attached image for layout of the current shunt section.For the TVS diodes I was worried about leakage as well, however I am not sure exactly how much leakage there will be since the datasheet doesn't give values for voltages less than VR. What I do know is that the SMF15CA TVS diode is specified to have a leakage current of 1 uA at its rated voltage of VR = 15V. Since the current section has a maximum of 5V across it, then I am anticipating that the leakage will be much lower than the 1 uA rated at 15V.Regarding the power supplies and common mode noise, do you see a potential problem with the design, or something I should investigate? Potentially it may be worth adding add some common mode chokes at the power inputs?Thanks again for your thoughtful response! This gives me a lot to think about and look into for further enhancements before I pull the trigger on buying boards.

author: derZockerMP
author_rank: Regular Contributor
timestamp: July 20, 2025, 04:48:57 pm
content: I think the C0G dielectric ceramics can be fitted. Only microphonics could be a problem with ceramics, but I wouldn’t worry about that too much.Yes, headroom is fine. Don’t forget about it for the current tooDid you simulate the oscillation stability of the current source?I would leave the filter in with 22k and 220k and test it out. In the worst case, you can experiment with the values in real life to find the perfect values and configuration.I think you could try your approach with heating the entire board. But insulation may be required. You can measure the TC with heaters on and off and compare the two values. Then you’ll have a rough idea of what your heater is capable of. In the worst case, you get more thermal hysteresis with the heater than without it. But that’s something you have to try out.I would leave the shunt in and test it in the first prototype. What I also came across is that you should star-ground important ground return nodes. Especially with the 1A current flow in the ground plane, there can be a high error due to this.TVS diodes should be good for you. If you're interested in the leakage, the only way is to measure the value yourself and select the low-leakage ones.Common-mode leakage is a current that is coupled in by the capacitance between the primary and secondary of your mains transformer. That can flow over your output test leads and create a voltage drop. Marco Reps did an interesting video about it:When it comes to programming, be careful with the low SPI frequency of the DAC1220. I also stumbled into that and lost two days trying to find the issueBest regards,Stefan

author: Kleinstein
author_rank: Super Contributor
timestamp: July 20, 2025, 06:04:23 pm
content: With the parallel connection of the SMD resistors one would add some copper trace to the resistance. If the resistors are very close to each other they would share the cooling part. The power per resistor is than misleading. Already with just a a single 1206 size resistor 100 mW is quite some power and the resistor would get somewhat hot. With maybe 70 K temperatue rise at nominal power this could still be around 30 K of temperature rise.For good precision it really makese sense to use a higher power shunt with 4 constacts / wires. These usually come as THT parts to be mounted with a heat sink. For the high current aready 1 V across the shunt is a lot. Usually less voltage (like 100 mV) gives better accuracy.A good shunt resistor is one of the more expensive parts.Isabellenhütte PBV ones sometimes come up on Ebay or similar.p.s. for the heater it could make sense to use the MOSFET as the main heat source. This would give a linear controlable power and there is no 2nd heat source with the FET. If needed to spread the power one could have a few channels in parallel.

author: Cpuch22
author_rank: Contributor
timestamp: July 20, 2025, 08:03:38 pm
content: Thanks Stefan for the additional advice.I went ahead and adjusted the voltage divider on the current generator input to give it a bit of headroom to account for calibration and offset 26 mA. Not sure if that's enough or not though. I also updated to filters from 1kHz down to 100Hz and by changing the 1.2k/22k resistors to 12.1k/221k.Thanks for sharing the MarcoReps video on common mode leakage. I remember watching it when it came out, but might need to watch it again as I don't quite remember everything he discussed.Also thanks for the tip on the DAC1220 SPI frequency. From the datasheet it looks like the max SPI clock period is (5+5)*Crystal period. So with a 2.5MHz clock, that would be 250kHz. Am I reading that correctly? I was potentially going to use 100kHz for the SPI clock. since this is pretty much DC I will be sending relatively few commands to the DAC so slower communications speeds will probably be fine... What did you use the DAC1220 for?Stefan and Kleinstein,I appreciate your concern regarding the current shunt on the current generator circuit I man need to research this some more... I did find this report from Vishay about temperature rise on thin film resistors (though the PTN series they reference seems to be rated for 400 mW vs 250 for the resistors I selected). For the 1206 sized component they saw a 46C temp rise at the rated power of 400mW. In their setup it looks like they had a 2 layer board with lots of thermal vias. Based on this report Im estimating maybe a 15-20C temp rise = 10ppm/C*15-20C = 150-200 ppm change.https://www.vishay.com/docs/60122/engineeringtestreport.pdfAlso I failed to take into consideration the resistance of the copper trace. Again estimating that the copper pour connecting the 10 resistors would potentially have 0.5mOhm or resistance = 500ppm...Regarding 1V being a lot for a current shunt, I was thinking that a higher voltage across the shunt would be potentially better since it would reduce the effect of offset, noise, and trace resistance, but I suppose its a balancing act with all the thermal related issues that arise as a result.Good point about just using the transistor standalone as the heater. Potentially I could use several of them spread across the board to get the distributed heating effect I was after. The resistor approach was easy in term sof layout since they are all in series.Lots of things to think about now. Appreciate all your your advice!

author: Kleinstein
author_rank: Super Contributor
timestamp: July 20, 2025, 09:38:56 pm
content: Yes there is the balance between the thermal effects and offsets / noise. There is not definitive answer as the power rating of the shunt is relatively easy to scale while super low offset gets increasingly tricky if the demands are very high.

author: Cpuch22
author_rank: Contributor
timestamp: July 21, 2025, 12:40:45 am
content: If I were were to potentially change up the current sense arrangement. Would it would be better to have switchable current sense resistors? Maybe 1 or 10 ohm for low current settings and 0.1 ohm for higher currents?I started looking at 4 terminal current sense resistors but I am a bit confused how to hook up the low side sense terminal with my current arrangement. Would I need to switch to a differential amplifier to take advantage of both sense terminals?

author: Cpuch22
author_rank: Contributor
timestamp: July 21, 2025, 02:28:32 am
content: Edit to my previous post. I suppose I could hook up the 4 terminal sense resistor in a 3 wire configuration with both low side terminals connecting to the ground plane. Or is there a better hookup method to do this?

author: derZockerMP
author_rank: Regular Contributor
timestamp: July 21, 2025, 05:12:38 am
content: I also used it in a reference source project and made some dev boards with it.https://www.eevblog.com/forum/metrology/dac1220-ref-schemtaic-10v/msg5789265/#msg5789265If you need some TC data of the circuit, let me know.You can hook the low side of the shunt to a star ground point where all important nodes are connected. The most critical ones are the DAC, voltage reference, and the non-inverting amplifiers. Not only the positive feedback path is critical, but also the negative one. When you have large currents, like 1A, in the ground plane, you can get a voltage drop of up to 1mV across the ground plane. To solve this problem, each important node is connected to a star point that is connected with a NetTie to the ground plane.Best Regards,Stefan

author: Kleinstein
author_rank: Super Contributor
timestamp: July 21, 2025, 07:20:18 am
content: The low side of the 4 wire shunt would be the point that links the power supply ground to the analog ground for the precision parts. Kind of using the shunt as the NetTie from power ground (e.g. ground plane) to star ground (precision ground).Ideally one would than use ground current compensation for things like the reference and other parts that give significan current to the star ground.It would make some sense to have more current shunts, though one might get away with slightly larger steps, especially for the lower current with possibly a bit more voltage at the shunt, like 0.1 ohm 10 ohm and 1 K. It is a compromise of cost vs performance though.

author: Cpuch22
author_rank: Contributor
timestamp: July 21, 2025, 08:35:25 pm
content: Stefan, pretty cool project! It seems like we are building similar devices. Would love to see how yours end up. Are you still working on it?I appreciate the tips about the sense resistor connections and values. I'm continuing to research how I want to handle that portion of the circuit and if I want to make any significant changes. Like you mentioned, it's probably going to come down to cost and complexity. More sense options is great, but increases the cost and complexity of the device. Lots of options to weigh, but that's part of the fun right?As always I appreciate all the advice!

author: derZockerMP
author_rank: Regular Contributor
timestamp: July 22, 2025, 05:18:52 am
content: Yes I'm working on a multifunctin calibrator that can handel 1V, 10V, 100V, 1µA, 10µA, 100µA, 1mA, 10mA, 100mA, 1A, 10Ohm to 10MegOhm Ranges and AC Voltages in Ranges form 0,7V to 70V. Still working on the schematic and layout. As a refrence I use a ADR1399 and a 20Bit DAC (AD5791). Also compliance limit detection and also some other handy features are implemented.Best Regards

author: Cpuch22
author_rank: Contributor
timestamp: July 22, 2025, 10:26:35 am
content: Wow that's pretty impressive! I'll be excited to learn more about how it progresses.What are you using for your controller? Programming is probably my weakest skill set so I'm using at ATMega so I can use the Arduino IDE. I was considering using a STM32 but got worried I would get stuck writing the software so I chickened out and stuck with something I've used a lot before.For the Ohms ranges are you using some kind of active circuitry with the DAC or precision resistors?

author: derZockerMP
author_rank: Regular Contributor
timestamp: July 22, 2025, 10:55:08 am
content: I'm using a Tennsy 4.0. It can also be programmed with the Arduino IDE. Programming is also not my prefered workThere are fixed precision resistors per decade form Vishay and Caddock build in. A impedance synthesizer would be to complex for this little room. Also some DMMs have a problem with such a circuit.Then the calibrator is in a working condition, I will make a sperate post. Also lots of validation have to be done first.Best Regards,Stefan

author: iMo
author_rank: Super Contributor
timestamp: July 22, 2025, 11:15:25 am
content: Quote from: Cpuch22 on July 22, 2025, 10:26:35 amMany STM32s are supported in the Arduino's IDE, so no worries..

author: derZockerMP
author_rank: Regular Contributor
timestamp: July 22, 2025, 06:16:33 pm
content: I quickly measured a SMA6J18CA TVS Diodes leackage current and come to 4,5pA at 4V and 45pA at 12V. So the real value is much lower (Typ 1µA).(Only measured by one device and don't know how this behave by aging)Best RegardsStefan

author: daisizhou
author_rank: Super Contributor
timestamp: July 23, 2025, 12:16:25 am
content: What is the frequency range of the AC part?

author: derZockerMP
author_rank: Regular Contributor
timestamp: July 23, 2025, 04:58:24 am
content: Thats unclear at the moment. Mut mainly its limited by the SPI Freuquency of the DAC. But 1kHz should be possible. So I think 50Hz, 100Hz, 500Hz and 1kHz would be a first thought.

author: Cpuch22
author_rank: Contributor
timestamp: August 02, 2025, 02:27:42 pm
content: Hi everyone,I have made some significant changes to the design from the post from a week or two ago based on everyone's helpful feedback on here. This required most of of the board to be re-routed. Attached is the updated schematic and some renderings of the board. Here are some of the main changes.- Changed +/- 12 DCDC regulator and +/-11 V linear regulator to +/-24V DCDC and +/-18V linear. This will give additional output range for the voltage generation section which will be software limited to +/-17V.- Revised some of the resistor divider ratios to give some additional output headroom for calibration.- Added dedicated buffer for DAC output instead of LPF.- Added analog switches to null the input of the unused section. i.e when voltage output is selected the current input will be nulled, and when current is selected the voltage input is nulled.- Added analog switches to the voltage output section so the user can configure 3 ranges: +17V range, -17V range, and 34V output range (using both +/- 17V outputs). The thought is I could have 3 separate scaling/calibration factors for these in software.- Revised the layout of the current generation circuit to minimize errors caused by thermal effects and copper resistance (still using 10x 10 ohm resistors in parallel) and changed the output transistors. The Heatsink now goes over the resistors and power transistors.- Revised the heater circuit to use only the transistor as the heating element. The transistor is located on the bottom side of the board directly below the voltage reference and will attempt to stabilize the temperature of that component/area of the board. I don't like having components on the bottom side of the board, but this seemed like the best way to handle that situation.- Changed the relays to latching type.- Added a big common mode choke at the dc power input to reduce effects of common mode noise/leakage from the external power supply. There is no choke on the USB input since this was designed to be powered from a USB battery power bank.- Added some additional circuit protection features.- Some updates were also required for the front display board due to the changes mentioned above.

author: Cpuch22
author_rank: Contributor
timestamp: August 02, 2025, 03:26:01 pm
content: Some of the 3D rendering photos didn't show up in my previous post so here they are.One other note is the 4 layer board stackup is: layer 1: Sig/Pwr, Layer 2: Gnd, Layer 3: Gnd, Layer 4: Sig/Pwr. In earlier revisions I had ground fill on the top and bottom layers in addition to the layer 2/3 ground planes, but I am not sure if this was necessary so I removed them. Any thoughts on if this was a good/bad idea? There are sill some ground polygons on the top layer around the voltage regulators, most notably on the return path for the current sense seen in the image on the previous post.

author: Kleinstein
author_rank: Super Contributor
timestamp: August 02, 2025, 08:25:31 pm
content: The parallel connection for Q2+Q3 would not work. Current sharing tends to not work so easy. Better use 1 larger transistor.

author: Cpuch22
author_rank: Contributor
timestamp: August 02, 2025, 10:51:24 pm
content: I suppose I could use individual source resistors to help force current sharing, but I suppose you are right it might be easier just to have a single mosfet.

author: daisizhou
author_rank: Super Contributor
timestamp: August 02, 2025, 11:09:07 pm
content: Why isn't Y1 placed in the middle?It seems to me that placing Y1 on the side may cause frequency shift or interference.Also, Q1 R15 F3 cannot be placed on the front? If you place it on the back, it may affect the use of hot plate heating installation.

author: Cpuch22
author_rank: Contributor
timestamp: August 03, 2025, 12:08:05 am
content: I'm not sure I understand the issue with Y1. Y1 is the 2.5MHz crystal oscillator for the DAC. It is off the the left side (about 8 mm) to keep it away from the sensitive analog signals/components on the right.The components on the bottom are the heater. The intent of these was to stabilize the temperature of the Vref/DAC. I could put them off to the side of those components, but I think the heat transfer will be much better with the placed directly below. I will probably reflow the top side components and then hand solder the components on the bottom. Its not ideal.Another idea is to put the Vref/DAC on a simple mezzanine board that plugs into the main board. I could put the heater components on the top side of the main board, and then the mezzanine board with the Vref/DAC could seat directly on top of the heater transistor. That would be more work though, and I'm not even sure if the heater circuit will improve or degrade performance at this point.

author: daisizhou
author_rank: Super Contributor
timestamp: August 03, 2025, 12:22:14 am
content: Quote from: Cpuch22 on August 03, 2025, 12:08:05 amYou can check the PCB layout specifications. Generally, it is recommended to place the crystal oscillator in the center or as close to the center as possible.Otherwise, the waveform generated by the crystal oscillator is easily disturbed or the frequency changes unexpectedly.If it is a heating element, then it is correct.If a heating element is used for temperature compensation, would it be better to open a window on the PCB?

author: Cpuch22
author_rank: Contributor
timestamp: August 03, 2025, 02:57:16 am
content: Hmm I'm not sure if it matters about the distance of the crystal from the DAC. On TI's development board for that IC they have the crystal spaced pretty far away from the chip, the traces look to be maybe an inch and half in total.Another update:- On the current generator section: I added 1-Ohm source resistors to each power transistor. Hopefully they will help to balance the current through each device. They will also dissipate some of the power at the full 1A load.- Added an 85C thermal cutoff to the power transistors and will be mounted under the heatsink with them- Revised the layout for the current shunt- The current shunt resistors now get their own heatsink which is isolated from the power transistors and thus should be more stable thermally.Maybe I'm getting carried away.... But I'm having fun.

author: Kleinstein
author_rank: Super Contributor
timestamp: August 03, 2025, 09:03:11 am
content: The clock for the DAC should not be super critical as it is only about short time stability. So no need to go to the center of the PCB. One still needs the load capacitors for the clock and avoid a ground loop there to avoid coupling the µC clock. So the ground from the 2 capacitors to the DAC chip should not be shared with any other circuitry. The distance from the crystal to the chip is likely still OK, though a smaller enclosed area woul be preferred.

author: Cpuch22
author_rank: Contributor
timestamp: August 03, 2025, 10:16:48 am
content: I was thinking about the current source transistor again. It may be better just to switch out the 2x smd transistors I have for a TO-220 package that then gets bolted to the enclosure. That would allow the enclosure to act like a big heat sink and would probably work best for preventing temperature coupling of that device to the rest of the instrument. I may play around with that today.Regarding the crystal for the DAC the PN is ECS-25-S-1X, which is specified as a "series" crystal. I had not heard of this opinion before, but according to ECS this variant does not need load capacitors. On mouser there were only 2 options for 2.5 MHz crystals available. This was one of them.

author: Kleinstein
author_rank: Super Contributor
timestamp: August 03, 2025, 05:41:40 pm
content: Even if the crystal selected is marked as series and may not need load capacitors it would be good to have the option to also use a crystal with load capacitors. It depends on the chip if they can work with a series crystal.A TO220 power MOSFET would be the better option for power and cooling.The cooling on the shunt resistors (10x 10 ohms in parallel) is still not great. It is also not so clear how the ground is sense at the low side. With up to 1 A the routing on the ground side can be very relevant.

author: GigaJoe
author_rank: Frequent Contributor
timestamp: August 07, 2025, 02:30:19 am
content: usually i soldering a blinking led , so here my absolutely naive 2 cents:I wouldcompletely stay away from any switching PS. injecting noisedigital and analog separated power , optocouplers , ideally 10 ohm 100uF RC filter per each opamp in feedingV ref need a buffer , dac load on vref not a constant, I even would add a separate VR for Vref + buffer.voltage output need 4 wire, need to compensate loss to DUT, same for resistance , if plannedif output opamp like this , i would add transistor follower, at least , with common back feed , better proper output schematic unitcurrent sense resistors at least 2 range for A and mA, i would thermally glue it to some thermal mass , avoid thermal runaway , relay to switchim not sure about dac buffer + LPS, unless you pick follower with much less bias current, LPS gives you additional uncertainties over RCdidn't look at pcb, but ground and current flows , basically cornerstone for this

author: Cpuch22
author_rank: Contributor
timestamp: August 08, 2025, 02:26:54 am
content: Thanks again for everyone's feedback. I'm working on some more sweeping updates... Again... Revising most of the power section. It is still using switching converters (they are required for this design) but I am adding lots of filtering and will be careful with the layout.I decided to scrap the external USB power bank idea as a secondary power source in favor of an internal 1S rechargeable LiFePo4 battery pack with integrated charger. This should allow the device to be more portable without having to worry about having a power bank plugged in all the time. Attached is a block diagram of the new power setup since the schematic version is still in work.I'm a little confused about grounding for this design at the moment. Lots of suggestions from everyone on star grounding instead of large unbroken ground planes. My understanding was that large, closely coupled, unbroken solid ground planes offer the best current return path and lowest impedance for return. However I suspect much of that information is focusing on AC impedance, and not DC (resistance)? My understanding was the return current will flow directly under the supply trace resulting in the smallest loop area. With star grounding this advantage is lost. Or am I understanding this concept incorrectly? Maybe for DC this doesn't matter?A few other comments:isolated power is not an option but I will try to create a layout that will minimize this eI do not think the Vref needs a buffer. The DAC has a 100k Vref input impedance, and the Vref can output +/-10mA with 15 ppm/mA accuracy. With the 100k input impedance that results in .375 ppm which is small enough to not be a problem I think.DAC-out now has a dedicated buffer. I'm considering removing the LPF.No 4 wire mode is planned for this deviceI did revise the voltage output opamp circuit to be more stable in case a capacitive load is connected per the attached image.

author: daisizhou
author_rank: Super Contributor
timestamp: August 08, 2025, 03:12:59 am
content: Can your final solution really achieve the design goals of 10 uV and 1 uA?Because as a voltage and current reference source, I have not found any similar reference circuits such as LTZ1000.It seems that your solution is biased towards the DC part, and there seems to be no detailed introduction to the AC part.Anyway, I look forward to your update, come on.

author: Cpuch22
author_rank: Contributor
timestamp: August 08, 2025, 04:14:24 am
content: Haha, It almost certainly will not meet those goals. But I would like to see how much performance it can achieve when it is done. It has been a really fun and great learning experience for me so far and that's was the primary purpose. It will be fun to see how good, or bad, it ends up when it gets put together.

author: TERRA Operative
author_rank: Super Contributor
timestamp: August 08, 2025, 06:34:29 am
content: For the heater, could you route a wiggly trace to act as a heating element under the part to be heated?If you make cutouts in the PCB you can isolate it thermally and mechanically too. Maybe make a little 3D printed clip-on cover as well.

author: GigaJoe
author_rank: Frequent Contributor
timestamp: August 09, 2025, 10:23:59 pm
content: here is ground basic , some primitivism , 3K resistor are something that consume 3 ma , opamp , for example , 0.01 - copper lineso top are chain connected , and second a star connectedimagine you reference voltage output in the beginningso for 1st variant opamp ground 300uV OFF , for 2nd 130 uV OFFsecondly: it a noise - imagine that opamp doing something , so ground current flow to the last opamp became variative that basically noise ...for a digital part it x1000 worse , microcontrollers or logical elements consuming significantly different , depend what are they doing\state etc ... so it paramount to divide completely analog and digital ground, and power supply ..... so ideally optocouples between DAC and microcontrollers, and a separate power supply for analog and digital part.technically you can achieve 10 uV pAI may suggest not all in one , but modular , block PSU, block Vref block voltage , block current ...consider you screwup on current - redo only this boardi'm not sure about TLV888 , due to Gain bandwidth: 14MHz , Slew rate Gain = 1, 10V step 40 V/µs , it's look great , but may oscillate , for this project something like BW 1 Mhz , 1 V/µs , would be more appropriate like OPA177 , OPA186 , 188, 189 ,180you may consider REF54250 , drop heater

author: Cpuch22
author_rank: Contributor
timestamp: August 10, 2025, 03:05:10 am
content: Thanks for the feedback Joe!I did switch the opamps to OPA2189 & OPA189 yesterday actually and have been reworking all the power, adding a second LDO for the digital circuitry. I was considering moving the DAC and Vref to a separate analog board that plugs into the main board, like you were suggesting. Its a little less risk just like you mentioned. If there's an issue with the main board I don't have to remake the whole thing. Maybe I could move all the analog components to a separate daughter board.For the star ground concept, how would that work with a dual supply, since there's no gnd connection for the power, would the decoupling caps return also be routed to the star ground? It seems counterintuitive to route gnd traces like that. From everything I have learned a plane/multiple planes would provide the most direct and lowest impedance/resistance return path? Its my understanding that return currents follow the same path as the supply trace, so having an unbroken ground plane (on layer 2) that's very closely coupled to the layer 1 supply trace, should minimize the loop inductance. I think the key to making it work is ensuring the layout is done well so that various parts of the circuit are essentially in their own sections so that currents from the digital/switching section do not cross currents flowing in the analog section. I think I need to study this topic more...

author: Kleinstein
author_rank: Super Contributor
timestamp: August 10, 2025, 06:47:02 am
content: The OP-amp choice is usually not that critical. The TLV888 looks like a low cost variant of the OPA189. If one wants it slightly slower there is the OPA182 with "only" 5 MHz GBW and lower supply current, which can be a plus for less heat. Another reasonable choice could also be the MCP6V51.For the ground it makes sense to have a type of power ground that could be from a ground plane and a separate precision ground as ref. point for the analog part. The precision ground should be routed as from a star ground, at least those parts that have current - just an OP-amp input may get away without. The decoupling would normally go to the power ground. It would only be very sensitive parts that don't produce interference that may also use the precision star ground. One should than have some impedance (e.g. 10 ohms range resistor or ferrite bead) in the supply to not couple supply ripple to ground. This can be a good idea for other parts too.There is than 1 link from the power ground to the precision ground - this could be at the voltage regulators or at a part like a ADC or DAC that has no good separation between supply and signal ground.For the DC analog part it is not about loop area, but about not sharing traces to the ground point. The loop area part is relevant for higher frequencies and digital parts.

author: iMo
author_rank: Super Contributor
timestamp: August 10, 2025, 07:24:54 am
content: Grounds are a problem when chasing uVolts, TCs, etc. Therefore I made myself the models of a "wire" and of a "pcb track" in the LTspice, thus I can see directly what is going on.https://www.eevblog.com/forum/metrology/ltspice-traces-and-wires-resistance-and-tempco/msg4687136/#msg4687136

author: Cpuch22
author_rank: Contributor
timestamp: August 10, 2025, 03:16:39 pm
content: Thank you for the tips about the grounding setup, it is making a lot more sense now. I have some time to work on the project today so I'll see what I can come up with.Joe had mentioned isolation so I have been thinking about that as well. It would require some significant changes to the whole design (again - hah!). Attached is a potential power setup showing the isolated configuration with how I think the star ground should be set up. I also added a separate 3.3 V supply for the current generation. Since the DAC and Vref are on the 5V supply I thought that potentially having the 1A supplied from a different source could help to eliminate errors. The lower supply voltage will help to reduce power dissipation as well.Stefan, regarding supply ripple; each switching power stage has filtering on the outputs and is then followed by a low noise LDO with high PSRR and a lot more filtering, I suppose I could add some additional chip ferrites to the power inputs of each analog component though.

author: GigaJoe
author_rank: Frequent Contributor
timestamp: August 11, 2025, 12:46:32 am
content: if you look at more closely to DAC1220 , you will see , DGND ,AGND - separated analog and digital ground, same for positive power .drop any switching power converters, basic transformer , bridge, LM317 \ 3378\ and capacitors , do not need fancy switching isolating PS ...do independent transformer for digital , and analog - very simple.and positive and negative output "" , it just a matter of swap wire , why headache for additional inverter ?, put relay instead ...in your schematic 1A ground current output linked with DAC ground, and precision V output ground , i recommend to make perfection for just voltage part , then you can add current stage later

author: Cpuch22
author_rank: Contributor
timestamp: August 12, 2025, 12:48:58 am
content: Hi all,Another update after getting to work on the design this weekend some. Attached is the updated schematic. Ignore the last (microcontroller) page for now since that still needs lots of updates such as the optocouplers etc for the digital signals that cross into the isolated area.Stefan thanks for the tip about the OPA182. They are a bit cheaper and almost the same in terms of offset and other performance metrics, and you are right I don't need the 14 MHz bandwidth of the OPA189.Joe, one of the main design criteria was for it to be small portable and able to be battery powered so having a mains transformer would not work for this design. It would simply it considerably though.The main updates are:- Split the schematic into more sheets to make it less cluttered- Power section has be completely redone. It now has isolated power supplies for each rail that supply the LDO regulators analog section similar to the block diagram I posed a few days ago with a few tweaks.- Added internal LiFePo4 batter and battery charger as 2nd power input and pushbuton controller- Small tweaks to analog and REF/DAC sections, updated opamps, removed LPF- Removed HeaterTo do- I still need to look into the star grounding setup for the critical analog traces.- Work on microcontroller schematic, add digital isolators- Redo the layout