MCP4922 DAC and MCP3204 ADC ground pins. Where to connect them ? - Page 1
Forum section: electronics / beginners

author: lukasz.kostka
author_rank: Contributor
timestamp: October 16, 2019, 07:07:24 pm
content: HI.I'd like to create a daughter board with DAC, ADC and reference voltage. I have a problem where to connect ground pins.Datasheetfor 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 ?

author: exe
author_rank: Unknown
timestamp: October 16, 2019, 09:00:16 pm
content: 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.htmlRelevant excerpt from there:Quote

author: lukasz.kostka
author_rank: Contributor
timestamp: October 16, 2019, 09:09:16 pm
content: 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 ?

author: lukasz.kostka
author_rank: Contributor
timestamp: October 16, 2019, 10:02:10 pm
content: And I can not connect at some cpoint on my daughter board two ground planses, because I will create a groud loop. Right ?

author: T3sl4co1l
author_rank: Super Contributor
timestamp: October 17, 2019, 03:12:50 am
content: 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

author: capt bullshot
author_rank: Super Contributor
timestamp: October 17, 2019, 06:21:24 am
content: Quote from: lukasz.kostka on October 16, 2019, 09:09:16 pmDon'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.

author: capt bullshot
author_rank: Super Contributor
timestamp: October 17, 2019, 06:25:10 am
content: Quote from: lukasz.kostka on October 16, 2019, 10:02:10 pmNot 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).

author: Kleinstein
author_rank: Super Contributor
timestamp: October 17, 2019, 07:14:46 am
content: 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.

author: lukasz.kostka
author_rank: Contributor
timestamp: October 18, 2019, 12:24:19 am
content: 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 ?

author: T3sl4co1l
author_rank: Super Contributor
timestamp: October 18, 2019, 05:11:58 am
content: 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

author: capt bullshot
author_rank: Super Contributor
timestamp: October 18, 2019, 09:16:35 am
content: Quote from: lukasz.kostka on October 18, 2019, 12:24:19 amYes, 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.

author: lukasz.kostka
author_rank: Contributor
timestamp: October 18, 2019, 06:38:29 pm
content: Thx. For information. This is what I came with so far.