Hi all,

I have been working on ADC and DAC, and I have buffer stage before the ADC and after the DAC, and also have micro controller. So, I have power-up the micro controller with the +3.3V, ADC and DAC with +5V and buffer stage with the +12V and -12V. So, my question is that, Shall I provide/connect the same ground to all power levels?. (or) Do I need to separate the grounds?, if so, what are the grounds to be separated?.

 

Hello there. The AGND pin of the data converter is connected to the
analog ground plane,and the DGND pin is connected to
the digital ground plane.The digital currents are isolated
from the analog ground plane, but the noise between the
two ground planes is applied directly between the
device’sAGND and DGND pins.The analog and digital
circuits must be well isolated. The noise between AGND
and DGND pins must not be large enough to reduce
internal noise margins or cause corruption of the internal
analog circuits.
It is a well-known fact that digital circuitry is noisy.
Saturating logic draws large, fast current spikes from its
supply during switching.Analog circuitry is quite
vulnerable to noise. It is not that the analog circuit
might interfere with the digital logic. Rather, it is possible
that the high-speed digital logic might interfere with the
low-level analog circuits. So the concern should be how to
prevent digital-logic ground currents from contaminating
the low-level analog circuitry on a mixed-signal PCB.
There are two basic principles of electromagnetic com-
patibility (EMC):
1. Currents should be returned to their sources locally and
as compactly as possible. If not, a loop antenna should be created.
2. A system should have only one reference plane, as two
references create a dipole antenna.
Designers think only about where the signal current flows
and ignore the path taken by the return current.
The high-frequency signals have a characteristic of following the path of least impedance (inductance).
The path’s inductance is determined by the loop area that the path encloses. The larger the area that the current has to travel to return
to the source, the larger the inductance will be.
The smallest inductance path is directly next to the trace.
So, regardless of the plane power or ground the return current flows on the plane adjacent to the trace. The current spreads out slightly in the plane but otherwise stays under the trace.

 

Ah yes, ADC and DAC and grounding,
Yes is the answer...

I say this as there are two , both valid schools of thought,
a) connect al the grounds together as one,
b) keep a the grounds separate , back tot he "star" point.

If you follow (a) blindly then you will end up in trouble,

unfortunately
(b) is all but impossible, and if you follow it blindly will end up in trouble !

Not much help am I so far.

The "trick" is to think like current.
And to remember that your aim is to stop noise of one system affecting the other.

i.e. ,if the system is a 24 bit ADC you would behave very differently to if its a 8 bit ADC,

Advice,
sorry, no matter what I say, you are going to get 1001 peopel arguing that is worng, the only way is X, which others will then argue about.

Some links , as you see its a hot topic, going back to the start of time ( well digital and analog circuits anyway )

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

https://www.analog.com/en/analog-dialogue/articles/grounding-again.html

https://www.analog.com/media/en/training-seminars/tutorials/MT-031.pdf

http://www.sigcon.com/Pubs/edn/multipleadc.htm

 

One of the most influential people in PCB design is Rick Hartley.

He is a consultant for EMI problems in PCBs that has worked for world leading companies

This seminar is on proper grounding -

 

As "Click_Here" mentioned, Rick is the industry expert on the subject and he is also a personal friend of mine and we've known each other for over 20 years. As was mentioned also, there are 2 schools of thought on this and both can be right and wrong. I have been designing PCB's for 30+ years and done AGND and DGND's both ways for different reasons. I'm not an expert at everything and I can prove it, but you're on the right path so far. The basic idea is like mentioned, keep the digital return path currents out of the analog returns. If your layout is placed such that you can have all digital signals on the digital side of the device and the analog circuits on the analog side of the device, you can have a single plane and shouldn't have any issues. That said, by-pass and de-coupling caps need to be located as close to the device as possible and of the correct values based on the logic or edge rate of the digital signals, typically they are very fast these days so .01uF and .001uF are good places to start. As was mentioned, you need to think like a return path field and understand that you don't want fields from one side to cross or mix with the other. If you can do that, you shouldn't have any issues. If you do split the planes, you tie them under or as close to the ADC/DAC as you can since that is the one place the currents will be connected so to speak. Effectively creating a separation between the AGND and DGND. If you place any of the digital parts on the analog side of the split, or visa versa, don't even bother with the split, you are going to have issues. These are the words Rick would use, "if the 2 signal types, (Analog and Digital) are not next to each other, they have no reason to talk/interfere with each other, therefore why do you need a split?" Use caution when referring to application notes telling you how to connect grounds and such, they don't always have your design in mind and can sometimes do more harm than good. (Don't get Rick started on App notes either. ) So to one part of your question "power the micro controller with the +3.3V, ADC and DAC with +5V and buffer stage with the +12V and -12V." I say this, they will all tie at some point. If you have a single power input to your design, I would ensure the power to the buffers stays over the same plane, (area) as what it is powering, like the +/-12V should stay on the analog side and the 5V also if it's the analog 5V buffer side, etc. The currents running the analog side will be returned to the power supply of the analog devices and same for digital. It's easy to see how the two sides can get intermixed without even realizing it so placement on your layout is really important. Been there, done that... Not pretty sometimes... :-(
Anyway, without seeing your layout or knowing if you are working on a PCB or bread board, it's hard to tell if what you have is good or bad. Just take what you read here and above, which I might add is some of the better advice I've seen on this, and review what you have and go from there. Oh, and splitting can be used best for really high input impedance circuits or instrumentation amps etc. where sensitivity can be a big factor. Good luck on your project.

 

As "Click_Here" mentioned, Rick is the industry expert on the subject and he is also a personal friend of mine and we've known each other for over 20 years. As was mentioned also, there are 2 schools of thought on this and both can be right and wrong. I have been designing PCB's for 30+ years and done AGND and DGND's both ways for different reasons. I'm not an expert at everything and I can prove it, but you're on the right path so far. The basic idea is like mentioned, keep the digital return path currents out of the analog returns. If your layout is placed such that you can have all digital signals on the digital side of the device and the analog circuits on the analog side of the device, you can have a single plane and shouldn't have any issues. That said, by-pass and de-coupling caps need to be located as close to the device as possible and of the correct values based on the logic or edge rate of the digital signals, typically they are very fast these days so .01uF and .001uF are good places to start. As was mentioned, you need to think like a return path field and understand that you don't want fields from one side to cross or mix with the other. If you can do that, you shouldn't have any issues. If you do split the planes, you tie them under or as close to the ADC/DAC as you can since that is the one place the currents will be connected so to speak. Effectively creating a separation between the AGND and DGND. If you place any of the digital parts on the analog side of the split, or visa versa, don't even bother with the split, you are going to have issues. These are the words Rick would use, "if the 2 signal types, (Analog and Digital) are not next to each other, they have no reason to talk/interfere with each other, therefore why do you need a split?" Use caution when referring to application notes telling you how to connect grounds and such, they don't always have your design in mind and can sometimes do more harm than good. (Don't get Rick started on App notes either. ) So to one part of your question "power the micro controller with the +3.3V, ADC and DAC with +5V and buffer stage with the +12V and -12V." I say this, they will all tie at some point. If you have a single power input to your design, I would ensure the power to the buffers stays over the same plane, (area) as what it is powering, like the +/-12V should stay on the analog side and the 5V also if it's the analog 5V buffer side, etc. The currents running the analog side will be returned to the power supply of the analog devices and same for digital. It's easy to see how the two sides can get intermixed without even realizing it so placement on your layout is really important. Been there, done that... Not pretty sometimes... :-(
Anyway, without seeing your layout or knowing if you are working on a PCB or bread board, it's hard to tell if what you have is good or bad. Just take what you read here and above, which I might add is some of the better advice I've seen on this, and review what you have and go from there. Oh, and splitting can be used best for really high input impedance circuits or instrumentation amps etc. where sensitivity can be a big factor. Good luck on your project.

Hi PadMasterson,

Thank you. Still I have some questions.

For example,
1) Shall I connect like like this or not?: one of the component of 3.3_VCC_Ground is connected to Analog Ground and the same component of 3.3_VCC_REF_Ground is connected to Digital Ground.
2) If the DC-DC converter is not isolated the primary and secondary, then, shall I connect the primary ground to the Analog Ground. And, secondary ground to the Digital Ground?.

 

Pinkyponky, As far as the first question goes, it would depend on the device you are talking about. Is one a reference for a specific part of the circuit or the other? Hard to say without knowing the device and it's purpose. For #2, what is the reason for the converter, powering digital or analog devices? Typically a converter is used to power one or the other or if it provides power to another regulator for another voltage, etc. so it may not make a big difference, but the key factor on ANY switching converter is to keep the input return paths separate from the output return paths. Very much the same as keeping analog from digital, etc. Doing that will ensure you have good stable and quiet converters along with keeping part placement tight and pay attention to those returns. If you can provide a bit more on that devise in your first question, that might help more.

 

Hi PadMasterson,

Thank you. Still I have some questions.

For example,
1) Shall I connect like like this or not?: one of the component of 3.3_VCC_Ground is connected to Analog Ground and the same component of 3.3_VCC_REF_Ground is connected to Digital Ground.
2) If the DC-DC converter is not isolated the primary and secondary, then, shall I connect the primary ground to the Analog Ground. And, secondary ground to the Digital Ground?.

I cant seem to find out how many bits your ADC / DAC are or the bandwidth / sampling speed.

Unless we know that,
we can but guess as to what measures you should use,
By default I'd say just wire the lot together on one plane,

 

Hello there. The AGND pin of the data converter is connected to the
analog ground plane,and the DGND pin is connected to
the digital ground plane.The digital currents are isolated
from the analog ground plane, but the noise between the
two ground planes is applied directly between the
device’sAGND and DGND pins.The analog and digital
circuits must be well isolated. The noise between AGND
and DGND pins must not be large enough to reduce
internal noise margins or cause corruption of the internal
analog circuits.
It is a well-known fact that digital circuitry is noisy.
Saturating logic draws large, fast current spikes from its
supply during switching.Analog circuitry is quite
vulnerable to noise. It is not that the analog circuit
might interfere with the digital logic. Rather, it is possible
that the high-speed digital logic might interfere with the
low-level analog circuits. So the concern should be how to
prevent digital-logic ground currents from contaminating
the low-level analog circuitry on a mixed-signal PCB.
There are two basic principles of electromagnetic com-
patibility (EMC):
1. Currents should be returned to their sources locally and
as compactly as possible. If not, a loop antenna should be created.
2. A system should have only one reference plane, as two
references create a dipole antenna.
Designers think only about where the signal current flows
and ignore the path taken by the return current.
The high-frequency signals have a characteristic of following the path of least impedance (inductance).
The path’s inductance is determined by the loop area that the path encloses. The larger the area that the current has to travel to return
to the source, the larger the inductance will be.
The smallest inductance path is directly next to the trace.
So, regardless of the plane power or ground the return current flows on the plane adjacent to the trace. The current spreads out slightly in the plane but otherwise stays under the trace.

@Delta Prime is right, but I'm going to come at some of it from another angle-- (I find when learning, multiple perspectives are best)-- 'noise' is voltage. Current is energy. In order for you to have a standard reference, the grounds must be connected one way or another, so that the +3.3 and +5 are relative to one another from the same reference. Digital electronics pull current in fits and starts based on demand causing voltage to bounce up and down inversely- a bypass capacitor usually makes this possible because it can supply this minute current spikes faster than the power-supply. However, this leads to digital 'noise' usually over several millivolts on the ground plane. Unless the analog signal you're trying to 'catch' is under that threshold (and you can use a scope to see what that threshold is), you'll be OK, because ADC usually has a sample-on-hold aspect. Put a bypass capacitor across both Vcc & Gnd and AVcc and Gnd.

I recommend looking at 'active filters' (and there are 'cookbooks' out there) to see if you can reduce that noise. As always in any _engineering_ discipline, it comes down to just 2 things: Identifying constraints you can work with in, and artistically satisfying those constraints in elegant and robust ways.

Some materials that may help:

The Art of Electronics 3rd Ed.
Author(s) Horowitz & Hill
ISBN-10: 9780521809269

Inductance Calculations
Author: Frederick W. Grover
ISBN-10: 048647440-2

Reference Data for Engineers: Radio, Electronics, Computers and Communications; 9th Ed,
Author: Mac E. Van Valkenburg
ISBN-13: 978-0750672917
ISBN-10: 0750672919

Active Filter Cookbook; 2nd Ed.
Author: Don Lancaster
ISBN-13: 978-0750629867
ISBN-10: 075062986X

 

The thing I found bad in Art of Electronics, they show every circuit earth grounded, going by the symbol anyway!