I want to measure a DC voltage with very high resolution (uV) and send the value to a PLC (based on an Arduino Mega.) Initially I selected an ADS1115, but I got some power noise due to loop currents (discussion in this question). I decided to replace this ADC by another of higher resolution (ADS1219) but I got similar noise as before. I think that the reason could be that both analog/digital grounds are connected on the ADS1219 evaluation board (explained in this question).

As a visual reference, find the following image of possible ADS1219 breakboard (found in here) which does not separate the grounds:

enter image description here

To avoid the evaluation board, I am designing a new board with an ADS1219 where I will separate the grounds. These are my questions:

  1. How do I connect each ground to the rest of the circuit? My idea is to separate both analog and digital parts and include a new connector to have both AGND and DGND, like this image modified by myself but based on the reference circuit mentioned above:

enter image description here

  1. Do the analog and digital ground/paths need special design at PCB level? That is, do they need separated ground planes? Do the traces need to be special, or it is just normal connections as AVDD and DVDD?
  2. Does it make sense to have a digital isolator for the I2C communication? As commented in here it helped a lot with the ADS1115, but I am not sure if it makes sense for the ADS1219 if I separate the grounds.
  • 3
    \$\begingroup\$ Separating grounds is almost always folly for EMC and other system-level purposes. Separation of current flows is best done in layout -- please show yours, and the connection of your board in the surrounding system (what ground references do the inputs and outputs have?). \$\endgroup\$ Commented Mar 17, 2023 at 3:17
  • 1
    \$\begingroup\$ "DC" "will not have EMC issues" -- could've fooled me with the I2C and active IC there but alright. ...Dear god, they put I2C interfaces on PLCs now? I...why? \$\endgroup\$ Commented Mar 17, 2023 at 12:51
  • 1
    \$\begingroup\$ What is your environment? Do you have typical industrial equipment nearby e.g. switches, relays, VFDs, uhh, process equipment, welding, heating, anything at all? Nearby might be say 10 meters or less; or more if sharing nearby mains branches. What about the rest of the system, what is the BTS connected to? What is the PLC connected to? And so on? \$\endgroup\$ Commented Mar 17, 2023 at 13:08
  • 2
    \$\begingroup\$ According to your diagram in your previous question, the battery looks like floating, but if it has anything else connected, it may have DC or AC reference to ground, your PC has DC reference to ground, and your 24V power supply may float or have DC reference to ground. It will be quite a task to start figuring out how the system really looks like, as your block diagram just has a couple of wires between boxes of unknown content. \$\endgroup\$
    – Justme
    Commented Mar 17, 2023 at 13:21
  • 1
    \$\begingroup\$ From what you have shown here, it looks like you are working at the wrong level - so to speak. Noise is not a problem you fix on the schematic level (unless you have something fundamentally bad going on - remember decoupling caps, etc.). Noise is an issue at the board design level - it is about where you place that cap, and how you route your traces. Unless you show a board design, then you are not going to get more than generalities and high level rules. \$\endgroup\$
    – Frodyne
    Commented Mar 17, 2023 at 14:57

4 Answers 4


To avoid the evaluation board, I am designing a new board with an ADS1219 where I will separate the grounds.

The datasheet shows why this is not going to work:

datasheet diagram

The red circle is around an electrical circuit between the analog and digital parts. Current flows between them. If the grounds are not connected, then you break that circuit and the device doesn't work. If you route the grounds a long distance before connecting them, that current sees a high impedance, which leads to voltage drop and thus noise. The line directly connecting them in the datasheet is to remind you that you must directly connect them as closely as you can.

The datasheet's recommended solution is pretty good

Here is what the datasheet recommends, with the analog parts of the chip shown in red and the digital parts shown in green.

enter image description here

Everything is over single ground plane, but since all the digital currents go down off the bottom, and all the analog currents go up over the top, they're effectively isolated from one another. This gives you a very low impedance connection between analog and digital ground while also making sure that ground currents don't cross between domains. You could be even more elaborate with ground cuts and star grounds, but this simple solution accomplishes the same thing.

What I would do

If absolute lowest cost is not a major factor, and you are ok spending an extra dollar per board, I would make VCC on your connector 5V and run that to the side of the board. I would then put a separate LDO (2 total) for both the analog and digital (on the appropriate half of the board of course) and generate separate clean 3.3V for both AVDD and DVDD right next to where it is needed. Finally, I would split the analog and digital lines into separate connectors, and put each on their respective ends of the board. That way analog ground currents don't meet digital ones at a connector. Finally, I would put one ground per analog line on the analog connector.

enter image description here

Note that a 25 cent part is fine for the digital LDO, and you don't need to buy a very high end part for the analog one either.

  • \$\begingroup\$ user1850479 I have some questions about your proposal: 1- Do you mean to use 2 LDOs, one for each part, and theen feed AVDD/DVDD separately?. 2 - By analog lines, you mean AINX and by digital lines you mean SDA/SCL? 3 - By end of the board, you mean the right end if the LDO is put on the left end? 4 - What do you mean by one ground per analog line? I will use only AIN0 and AIN1 in differential mode. \$\endgroup\$
    – bardulia
    Commented Mar 17, 2023 at 10:38
  • 1
    \$\begingroup\$ @bardulia I added a quick MSPaint drawing showing the orientation of parts and the direction of ground current. If you want you could twist differential pairs and use 1 common ground next to them, although two grounds would also be fine, 1 per half of the pair. \$\endgroup\$ Commented Mar 17, 2023 at 15:48
  • \$\begingroup\$ Thanks! one more question before implementing the pcb: I had also tried BOOSTXL-ADS1219, which is an evualuation board for ADS1219 datasheet: ti.com/lit/ug/sbau316/… does this board also have separated analog and digital similar to your proposal?. I would say that yes but I am not totally sure. \$\endgroup\$
    – bardulia
    Commented Mar 17, 2023 at 17:28
  • 1
    \$\begingroup\$ @bardulia Yes it does, and in fact that layout is very similar to what I drew above (but with only 1 LDO and additional 3.3V external rail). IMO this is the most logical way to layout the board, so likely most well designed implementations will be similar. \$\endgroup\$ Commented Mar 17, 2023 at 17:37

Do the analog and digital ground/paths need special design at PCB level?

Yes, the main problem is return currents causing common mode noise. The PCB ground has resistance, so if a current is returning on the ground it will create a voltage.

Another caveat is this will not be a problem as long as the voltage on the ground is the same on the sensor and the ADC

There are several options available to the designer to allow them to do this.

  1. Separating the digital and analog planes with a single grounding point between the two - This scheme makes allows the sensor and ADC to have the same ground. This has issues because usually a single grounding point is used between the digital and analog planes, which means that changing return currents between the analog section and the digital section will create common mode noise.

  2. Isolating the digital and analog planes - This scheme allows for a single ground for the analog section. It basically forces the ground to be at the same potential, all return currents go back to the isolated power converter so common mode noise from return currents are significantly reduced and RF from other sections of the board can be controlled via the isolating bridge. The problem with this scheme is it's expensive as several isolator chips are needed which adds to cost.

  3. Proper layout. The same objectives can be achieved with proper layout (I have been able to do nV ADC designs with this method) by separating the analog and digital sections but not allowing any switching or changing loads to have currents run through the ADC/Sensor section. Voltage regulators for the ADC's should be placed near the sensor section. Basically you can draw a line from the ground points of changing loads back to their voltage regulators and the main grounding connector (where all return currents flow back to) if that line runs through the ADC section then a voltage will be seen at the ADC. It doesn't take much current for this to happen.

Another thing you can do is estimate the copper ground between devices and try to model it, I find that tedious so I try and eyeball it.

A 10mA current running through 0.5mΩ ground plane (1oz copper sq) will be 5uV so that gives you an idea of what kind of currents can be a problem for a uV design.

How do I connect each ground to the rest of the circuit?

I would use the proper layout method, I prefer using that because it lowers cost, but if you are not conformable with this method the other methods might be better.

  • \$\begingroup\$ Due to the other answers, I will probably try your third method. Do I need one LDO for the analog part and another one for the digital part I guess?. \$\endgroup\$
    – bardulia
    Commented Mar 17, 2023 at 10:50
  • 1
    \$\begingroup\$ You can combine the grounds at the ADC with the third method \$\endgroup\$
    – Voltage Spike
    Commented Mar 17, 2023 at 23:31

In general, there are two schools of thought regarding Ground planes, to split or not to split. Some will say that you should split your analog and digital grounds, and join them at one point near the connection to the board power or point of generation. Thus you can force the return paths to be quite separate and reduce if not eliminate cross-talk.
Personally I dont do this. IMO the process of trying to separate the grounds, and manage the connection between them creates more problems than it solves. I've seen some quite iladvised layouts, cutting a layer's ground in two in order to do this, and this creates is a longer, more inductive path for ground currents to flow. Quite often chips connect thier two grounds internally anyway, making the question moot.

What I personally practice, is to manage the ground currents, where they must flow, and what they might couple into along the way. Think of the blocks below as a simplified PCB veiwed from the side Simplified PCB veiwed from side

In this 2D PCB, the analog signal is routed along the same path as both the digital currents and the ADC's power currents, providing plenty of oppourtunity for cross over. Even if the digital circuit is nowhere near, the power supply currents still have to make thier way back to the PCB, so if these current's pass the ADC input there's potential for noise. If I swap the blocks aroundsimplified PCB diagram

Now the analog circuitry is not exposed to any other currents in the ground path. This is obiously a pretty oversimplified example, but the principle applies to a 3D PCB. Remember that the return path will always be the lowest impedance path back to the point of generation, and then design your circuit so your return paths are seprated.

  1. Datasheet says AGND and DGND must be connected together, and they can't have much difference between them. It is not clear why they go separately to the connector, that will not help, and may even make things worse, depending on how they are connected on the other board.

  2. Datasheet says you can have separate digital and analog ground planes. But it also says the grounds must be tied together at the ADC. The point is that the GND or supply connections are not magical, they just need to be routed in a way that avoids digital currents affecting analog currents, and maybe filtering analog supplies separately.

  3. No, isolating I2C bus won't help. If you do isolate I2C bus, you need also provide isolated power supply to the isolated side from the non-isolated side.

  • \$\begingroup\$ Then maybe it would be better to use another type of ADC, one with fully separated grounds. Any recommendation about this idea?. \$\endgroup\$
    – bardulia
    Commented Mar 17, 2023 at 12:21
  • 1
    \$\begingroup\$ It will likely be more noisy, since you need to provide isolated power separately which is typically done via an isolated switch mode converter. It is not fully understood what is the source of your noise, if already multiple ADCs are noisy. Maybe you have noisy supplies, do you use a switch mode supply or regulator? Is the power coming from mains brick or battery? Are there ground loops you have not considered? \$\endgroup\$
    – Justme
    Commented Mar 17, 2023 at 12:24
  • \$\begingroup\$ By isolated switch mode converter, you mean a DC/DC converter?. Regarding the measurment, there is a Battery Test System (BTS) that injects constant current to charge/discharge the battery cell and simultaneously I measure in paralell the battery cell voltage with the ADC. Could this BTS create another ground loops?. Regarding supplies, I use an DC/DC converter to feed the ADC an an independent power supply for the PLC. \$\endgroup\$
    – bardulia
    Commented Mar 17, 2023 at 12:33

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.