Hello,
We will use ADS1158.
But we had confused about analog and digital ground.
Do we have to seperate them?
I did not see any information about that.
I though negative voltage can be applied to AVSS,because of that AVSS and DVSS is different isn't it?

 

When working with noise sensitive stuff like an ADC, read the datasheet and pay attention to any notes on layout.

Generally you want to keep your digital and analog grounds (and other traces) separated for noise reasons. Digital circuits tend to have a lot of noise from the digital parts switching on and off suddenly. Clock signals for the processor, digital communication interfaces like SPI, switching power supplies, etc.. These signals usually have square edges and are at frequencies that are easily picked up by nearby traces, including ground, and this can be a problem for your ADC. For example, if you are trying to take consistent ADC readings, but your ADC input lines have ripple voltage because they're picking up noises from nearby digital lines, then your ADC readings can be all over the place. It's also important to keep an eye on your ADC power lines, especially if you're using a switching regulator. One effective way to keep the digital noise out of your analog lines is to keep the digital and analog parts of the circuit as physically separate as possible, including grounds. At some point they need to come together, but the more you keep them separate the better.

You can also do a lot of noise filtering with capacitors, use different types and sizes depending on the frequencies you need to filter. Keep the caps as close to the devices that need the filtering as possible. For example if your ADC is getting too much noise through its power pins, don't put the caps way across the board, put them as close to the ADC pins as is physically possible. Good layout can make your life a lot easier when it comes to noise control.

 

If you just apply +5V and Gnd to the power of the Chip then you can see the figure 55 on the page 43 of ADS1158, you can see that there are three pins need to connected to the Ground, AINCOM, AVSS, DGND(post #1), and you have to separated three different Ground path to the terminal pins, and you also need to add a 0.1uF and a 10uF connected to +5V and Gnd of the terminal pins, and the two Caps as close as you can connected to the terminal pins.

 

Ideally you have a split ground plane with the analog ground part under the analog parts and the digital ground under the digital parts.
The grounds are then joined together at just one point under or near the A/D converter.

In my past job I was given a mixed signal PCB, to determine why the A/D converter digital word output had excessive noise.
Examination of the board showed that the board layout designer had misconnected the analog and digital ground pins of the A/D converter to the analog and digital ground planes .
Redoing the board with the correct ground connections solved the problem.

 

some point they need to

Ideally you have a split ground plane with the analog ground part under the analog parts and the digital ground under the digital parts.
The grounds are then joined together at just one point under or near the A/D converter.

In my past job I was given a mixed signal PCB, to determine why the A/D converter digital word output had excessive noise.
Examination of the board showed that the board layout designer had misconnected the analog and digital ground pins of the A/D converter to the analog and digital ground planes .
Redoing the board with the correct ground connections solved the problem.

Thanks for reply?
Could you share a bad connection example?

 

Could you share a bad connection example?

Anytime the analog and digital grounds have more than one common connection, you have a ground loop, with some of the digital ground currents going through the analog ground, causing analog ground-bounce noise
You always want to look at all the ground paths for all digital signal currents, and make sure they can't sneak through the analog ground.

 

Can someone clarify the point of connection for me. Why join grounds near the ADC?

I’d thought that all connections to ground on the ADC should have a capacitor to the associated power supply, at the chip. And where I’m confused is I’d connect the various grounds near their associated power supplies, not at the chip.

 

Can someone clarify the point of connection for me. Why join grounds near the ADC?

I’d thought that all connections to ground on the ADC should have a capacitor to the associated power supply, at the chip. And where I’m confused is I’d connect the various grounds near their associated power supplies, not at the chip.

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

 

Can someone clarify the point of connection for me. Why join grounds near the ADC?

Depends upon how much voltage difference the ADC can tolerate between the analog and digital grounds (ADS1158 value below).
If the ground voltage difference due to the various ground resistances and the two supply currents exceeds that value (0.3V in this case for the digital ground lower than the analog ground), it would be a problem.
Connecting the two grounds at the ADC eliminates that possible problem.

 

Board layout and power routing issues -

https://www.analog.com/media/en/tec...294542582256114777959693992461771205AN280.pdf

https://www.cypress.com/documentati...nd-psoc-5lp-mixed-signal-circuit-board-layout

https://www.nxp.com/docs/en/application-note/AN1259.pdf

https://www.nxp.com/files/training_pdf/WBNR_PCBDESIGN.pdf

http://cache.freescale.com/files/FTF_2015/ftf-acc-F1213.pdf

Out of curioosity any interest in an ARM UP with 20 bit A/D on it, + Vref and other
analog like OpAmps and muxes.....


Regards, Dana.

 

Capacitor technologies for bypassing big issue -

Regards, Dana.

 

 

You don't need fancy layouts to get good performance with a ADC but you do need a thoughtful layout even on a proto-board. With this junk-box design the analog and digital ground are joined at the electrostatic shield that separates the analog and digital sections of the circuit board.

https://forum.allaboutcircuits.com/threads/50nv-resolution.130468/#post-1073894

 

Depends upon how much voltage difference the ADC can tolerate between the analog and digital grounds (ADS1158 value below).
If the ground voltage difference due to the various ground resistances and the two supply currents exceeds that value (0.3V in this case for the digital ground lower than the analog ground), it would be a problem.
Connecting the two grounds at the ADC eliminates that possible problem.

View attachment 186338

Nsa's linked document shows the following image:

​

I find it interesting to note that both circuits are connected to ground via an RL filter. I'm guessing that's to dampen possible high frequency ringing. But the document itself does not mention that it's recommended to connect both grounds at the ADC. And I was of the same impression as DJS that the grounds should be connected at the power supply, although what you've mentioned makes perfect sense now that I think of it.

Question, if I were to connect both grounds as close as possible to the ADC, would the use of resistors and ferrites in series still be recommended?

EDIT: I just realized I asked a stupid question... those RL symbols are there to represent the resistance and inductance of the traces, and are not actual components, right?

 

Question, if I were to connect both grounds as close as possible to the ADC, would the use of resistors and ferrites in series still be recommended?

EDIT: I just realized I asked a stupid question... those RL symbols are there to represent the resistance and inductance of the traces, and are not actual components, right?

Right.
But you bring up a good point.
It may be a good idea to use a ferrite bead to connect the grounds near the ADC.
That will minimize any sneak path for the high frequency digital edge noise.
Also if you use the same power for both analog and digital, a ferrite bead between the two will also minimize noise crossover.

 

One of the most debated topic in PCB layout: split ground planes.

PREMISE: Everything that has been mentioned by previous post (e.g by @crutschow, @ScottWang and @MrSoftware) is 100% correct and valid. Star grounding is a good way to keep the noise coming from the fast switching signals of the digital part of the design to crosstalk to the analog part of your system.

However, there are cases when this is not the most suitable approach. An obvious case is for example when you have other mixed signals ICs, such as a digital potentiometer in your analog section. In this case you will need to route some traces across the two planes. It is not a good idea having traces crossing split planes (the EM emission can be quite significant). In these situations is much more preferable to partition your design in analog and digital without the use of a split plane. The reason is that the decay in space of noise generated by the digital lines can be quite space limited, avoiding its propagation to the analog part.

Here some references where you can better understand the concept of partitioning vs splitting ground planes:
http://www.ti.com/lit/an/slyt512/slyt512.pdf
http://www.hottconsultants.com/pdf_files/june2001pcd_mixedsignal.pdf