MCP4922 DAC and MCP3204 ADC ground pins. Where to connect them ?

[lukasz.kostka]

HI.

I'd like to create a daughter board with DAC, ADC and reference voltage. I have a problem where to connect ground pins. Datasheet for MCP3204 states on page 24 that both AGND and DGND should be connected to analog ground. I am confused, why separate pins on IC since they need to be connected to same ground plane ? DAC has only one GND pin. Where should I connect it ? GNDA or GNDD ?

[exe]

That's because an external trace has lower resistance than the internal connection. Designators such as AGND and DGND do not tell where the pins should be connected. They only tell where they are internally connected.

More details here: https://www.analog.com/en/analog-dialogue/articles/staying-well-grounded.html

Relevant excerpt from there:

Many ADCs and DACs have separate analog ground (AGND) and digital ground (DGND) pins. On the device data sheets, users are often advised to connect these pins together at the package. This seems to conflict with the advice to connect analog and digital ground at the power supplies, and, in systems with more than one converter, with the advice to join the analog and digital ground at a single point.

There is, in fact, no conflict. The labels, “analog ground” and “digital ground,” on these pins refer to the internal parts of the converter to which the pins are connected and not to the system grounds to which they must go. For an ADC, these two pins should generally be joined together and to the analog ground of the system. It is not possible to join the two pins within the IC package because the analog part of the converter cannot tolerate the voltage drop resulting from the digital current flowing in the bond wire to the chip. But they can be tied together externally.

[lukasz.kostka]

So DAC, ADC and reference voltage GND pins should be connected to AGND. Of course I need to place DGND under the SPI lines. Am I right ?

[lukasz.kostka]

And I can not connect at some cpoint on my daughter board two ground planses, because I will create a groud loop. Right ?

[T3sl4co1l]

If you don't have extremely specific requirements, and you don't have the skills to resolve a split-plane design -- better to simply pour ground over everything, and keep the digital to one side and the analog to the other side.

Tim

[capt bullshot]

So DAC, ADC and reference voltage GND pins should be connected to AGND. Of course I need to place DGND under the SPI lines. Am I right ?

Don't split GND to AGND and DGND. Use one GND for everything, and make a large GND plane over the whole board. Don't route digital signals through analog signal areas of the board.

[capt bullshot]

And I can not connect at some cpoint on my daughter board two ground planses, because I will create a groud loop. Right ?

Not connecting the planes can create large electromagnetic interferences. Better just use one plane for all. That's a fits 90% of use cases rule, exeptions may be applicable if you have an application with special requirements (e.g. very high stability - single digit ppm range) or high power (more than some 100W), or high voltage (more than some 100V).

[Kleinstein]

Unless one has very stringent requirements one can get a way with a single ground. The ADC and DAC listed don't look like high end - more like lowest cost.  How critical the ground is, also depends on how often data are send and read. With little trafic going on, there is no problem having the ground even at a sensitive point.

For the ground I would be careful with using ground pour (e.g. fill the rest of the board with ground). There is a good chance that ground pour gives a poor ground. A highly segmented / cut ground plane can be quite bad.
In a circuit that cares about ground one should more like route the ground part first and not use the left overs. One may still later fill the rest with ground too.

[lukasz.kostka]

Maybe I haven't stated my situation clear enough. Motherboard has two ground planes AGND and DGND. They are connected at some point on motherboard. Now, if I use one GND plane on my dayghter board, I will create a ground loop. Right ?

[T3sl4co1l]

Whelp, then that's forcing the complicated solution.

I would have to see both circuits and layouts to decide how to proceed.

The surest way would be to treat them as nearly isolated circuits: use differential amplifiers to sense the signal-to-its-ground voltage, transferring it to local ground reference for further processing.  Then you do not need to bridge grounds.

This is probably an over-the-top solution, but it's impossible to say without detailed information and analysis...

Tim

[capt bullshot]

Maybe I haven't stated my situation clear enough. Motherboard has two ground planes AGND and DGND. They are connected at some point on motherboard. Now, if I use one GND plane on my dayghter board, I will create a ground loop. Right ?

Yes, this creates a ground loop. Most often this doesn't do any harm to the system and still is the better choice than splitting the plane, but it depends on your particular case.

Having a single point star GND between analog and digital creates large amounts of noise if the circuitry is wide spread and has more then one point where signals cross the border between analog and digital. You'd have to route all traces that cross the border along that one connection point, or place all A/D D/A chips over that one connection point. The textbook example works for exactly one chip that crosses that boundary and the AGND/DGND connection is under the chip. If there's more than one chip involved, having AGND/DGND connected under each chip creates ground loops, but still is the better choice than having it connected under one chip. Best choice is to have a solid GND plane. So if you can't change the motherboard, improve its GND plane by making your board with a GND plane.

If can't avoid splitting the GND, connect all A/D and D/A chips (no matter if these are labelled analog or digital) to your analog GND. This reduces noise inside the chip. Now you have a lot of nasty digital signals crossing the AGND/DGND border, this makes up nice loop antennas. You can try to mitigate this issue by making the digital signals high impedance and slow - beware, now they work as receiving antennas for external EMI. So you'll have to additionally filter the signals. If you do this right, it may work. Or isolate them by using suitable isolators. If you connect the chip's GND pins to AGND/DGND as they're labelled, you've got the same issue, but within the chip and you can't do anything about it.
Having a solid GND plane solves this issue and maybe forms a GND loop with your mainboard. This may increase EMI issues on the mainboard, this depends on the circuitry and layout. Worst case is that you'd have to isolate your analog and digital parts to get it right, best case would be that the mainboard circuitry isn't harmed by your GND plane.

[lukasz.kostka]

Thx. For information. This is what I came with so far.