• State TI Thinks Resolved
  • Locked Locked
  • Replies 5 replies
  • Answers 2 answers
  • Subscribers 46 subscribers
  • Views 3018 views
  • Users 0 members are here
Support feedback
Options
Options
Similar topics

This thread has been locked.

If you have a related question, please click the "Ask a related question" button in the top right corner. The newly created question will be automatically linked to this question.

ADS1255: Designing a stacked PCB / Connecting analog and digital ground

Daniel Muell
Prodigy 140 points
Part Number: ADS1255
Other Parts Discussed in Thread: ADS124S08, ADS1256

Hi there i am new here.

First of all sorry for my bad english. At this moment i am developing a stacked PCB (I dont know if this is the right term for this thing. In general its two PCBs on top of each other and they are connected with pin headers). The two boards are powered by the same battery source. There are two voltage regulators.One one each board. I am using two layer PCBs.

On the first board there is all the analog circuit including the ADC. Also the 5V voltage regulator for the ADC (ADS1255) is placed on this board. The SPI of the ADC is going through the pin headers to the second board. Apart from the ADC there are no digital components on this board.

On the second board there is an atmel microcontroller, some periphrals and a bluetooth modul. Also a 3.3V voltage regulator for the digital circuit is placed on the second board. As the ADC also needs 3.3V for its digital part the 3.3V are connected from the second board through the pin headers to board one and the ADC.

On both PCBs the bottom layer is used as a ground plane. Because i am connecting the 3.3V thorugh the pin headers i also connect the GND of the 3.3V to board one where all the analog stuff is going on. The GND of the 3.3V could be seen as DGND because only digital components are supplied through this regulator.

Here comes the part where i am asking myself how to do it right:

There are a lot of opinions on how to connect the AGND and the DGND of the ADC together. A common method could be connecting AGND and DGND right at the ADC which is than the star point of the ground. As my two voltage regulators are powered by the same battery the two grounds are also connected at the battery. So the ADC cant be the ground star point. That would form a loop.

Others say to just use one big ground plane on the PCB where the ADC is placed. But as i am only getting my DGND to the analog circuit through the pin headers i thought it could be easy to keep AGND and DGND separated. But.... the datasheet of the ADC says:

" If a split ground plane is used with the ADS1255/6, make sure the analog and digital planes are tied together. There should not be a voltage difference between the ADS1255/6 analog and digital ground pins (AGND and DGND)."

So if i am getting it right the two ground planes of the 5V and the 3.3V supply can't stay separated. But on the other side i dont want to form any ground loops. Is there any recommended way to to it in case of such a sandwich PCB ? I've added a picture that shows the two PCBs in general. Where to connect the GND? Thank you very much.  

  • 0
    TI__Guru* 93985 points
    Daniel,


    I'm glad you're asking theses questions now as you are planning the layout. Too often, people think about this after they've built the boards, and already have problems.

    As you've described it, some say that you should lay out the board with an AGND and DGND and then star connect the two grounds under the ADC, others say that you should use a single large ground plane. I think both approaches work fine, but I like to think about the star connected separate grounds. It forces you to think about how the return currents will flow through the board. With large single ground plane, you count on the fact that your resistance to ground will be very low.

    Because you're connecting the boards through the pin headers, I would think of the ground at the pin headers as your star ground point. Lay down large traces for both AGND and DGND back to pin header for Board 1.

    As for other advice about the layout, there's a write-up in some of our datasheets about some layout guidelines. For some generic layout recommendations, you can look at the ADS124S08 datasheet and see what we've written:

    www.ti.com/.../ads124s08.pdf

    You'll find information on page 98 in the above datasheet.


    Joseph Wu
  • 0 in reply to Joseph Wu
    Prodigy 140 points

    Hi Joseph,

    first of all, thank you for your answer and sorry for the delayed reply. I'm glad to hear that my approaches were not completely wrong. I already bought the components and want to hand over the PCB for manufacturing as soon as possible.

    Joseph Wu said:
    Because you're connecting the boards through the pin headers, I would think of the ground at the pin headers as your star ground point. Lay down large traces for both AGND and DGND back to pin header for Board 1.

    You mean to run separate traces from ADC Pins (AGND & DGND) back to the Pin headers. But where should i do it. On the top layer or isolate the traces on the bottom layer from the general GND-Plane? And another quastion is, where to connect the battery cable. Probably as close to the pin header as possible?

    Joseph Wu said:
    As for other advice about the layout, there's a write-up in some of our datasheets about some layout guidelines. For some generic layout recommendations, you can look at the ADS124S08 datasheet and see what we've written:

    Thanks for the link. I think I've seen this figure somewhere while i was doing my researches. I now read the guidelines and they also recommend to split the grounds.

    I've created another beautiful picture which shows how i understand the ground connection you described.  I will explain it a little bit.

    Like before, there are the two PCBs with their pin headers. On board 2 there are all the digital components. On board 1 all the analog ones including the ADC. The SPI of the ADC is connnected through the pin headers to board 2. On the pin headers there are several pins for GND. They are marked as a red rectangle. On both boards the bottom layer (represented by the transparent blue rectangle) is connected to GND only at the pin headers. The negative pole of the battery is only connected to board 1 and then to the pin headers as shown. The positive pole is connected to the the voltage regulators on each board. All the grounds of  the components, except the ADC, are connected to the bottom layers through vias. The AGND and DGND of the ADC are not connected to the bottom layer. They are connected to the pin header GND with separate traces. Is that what you mean? If i dont have any obvious mistake the pin headers should be the star point. But if i will do it like this, is it guaranteed that AGND and DGND have the same potential? And how to connect the decoupling caps. Probably to the general GND-plane on the bottom layer right?

    Thank you very much.

  • 0 in reply to Daniel Muell
    TI__Guru* 93985 points
    Daniel,


    We've been talking a bit over here and I'm going to retract what I said about star grounding it back to the pin. Since you've got a simple analog board, with only the digital on the ADC, you should use a single ground plane. In the end, it's just more important to keep the analog and digital grounds the same, and not split them up at all. You'll still need to consider how the digital current returns to the ground, but as long as you have the analog and digital sections moderately separated, it should be fine.

    For the second board, it seems that you only have digital ground. In that case, it seems that the single digital ground plane will work fine being brought up through the header. Just make sure the connection from board to board is short and low inductance.


    Joseph Wu
  • 0 in reply to Joseph Wu
    Prodigy 140 points
    Thank you again for your answer. So i will undo my changes again :) I will do only one ground plane on each board an the two planes are than connected through the pin header. This way the return currents of the SPI can go through the pin headers and should not effect the analog circuit too much. What do you think in terms of ground loops. Is it better to connect the negative pole of the battery only to one board as shown in my picture or to both? I think if i connect it directly to both voltage regulators i will create a "nice" loop.

    battery --> 3V3_regulator --> GND-plane_2 --> pin_headers --> GND_plane_1 --> battery ... and the other way round, too. But if i dont do it all the currents of board 2 have to go back through the pin headers and than back to the battery. I'm confused.
  • 0 in reply to Daniel Muell
    TI__Guru* 93985 points
    Daniel,


    To keep things simple, we would generally send the battery power (and ground) to just one board and feed them up to the second board. That would probably limit any loop voltage in case there is any ground current flowing.

    If you look at some of our evaluation modules, we've often used a mother board and a daughter card. The ADS1256EVM for example has all power and digital on the mother board and the analog circuits + ADS1256 on the daughter card. That seems to work well in collecting clean data. If you're interested, you can look at the user guide and look at the schematic and daughter card layout:

    www.ti.com/.../sbau090d.pdf


    Joseph Wu