• State TI Thinks Resolved
  • Locked Locked
  • Replies 8 replies
  • Answers 3 answers
  • Subscribers 46 subscribers
  • Views 450 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.

Original question:

ADS1248: Schematic review for multiple 2-wire PT100 RTD measurement

ADS1248: Ground plane questions

Tony Steinbock
Prodigy 180 points
Part Number: ADS1248
Other Parts Discussed in Thread: ADS124S08

Hello TI-Team,

based on my circuit review post, I need some help with the layout. Basically, it is a board with 4 layers, wherein the following layers are used:

- Layer 1: Signal + Ground fill (component placement side)

- Layer 2: GND

- Layer 3: Power polygons + Ground fill

- Layer 4: Signal + Ground fill

Here is my current status:

There are 6 high-side switches on the bottom of the picture (the SOIC-8 parts), each switching 24V / 0.4A. The high-side switches partially pulse the voltage and are controlled with a PWM (f < 1kHz). The high-side switches (connectors) unfortunately have to be placed this way due to mechanical conditions. The 24V supply comes from the top left und goes on the left down to the high-side switches (actually drawn in the top layer, not in the power layer). There are two ADS1248s above the high-side switches, each handling 3 PT100 sensors. The microcontroller is located above the ADS1248.

My current approach was to separate the ground (top layer) between the high-side switches and the analog front end of the ADS1248 in the layout. Does this make sense or would it be better to use a complete ground plane - both in the top and in the ground layer?

  • 0
    TI__Mastermind 35241 points

    Hi Tony,

    I am looking into this and will get back to you in the next day or so

    -Bryan

  • 0
    TI__Mastermind 35241 points

    Hi Tony,

    It was not entirely clear from the description you gave, but if you are attempting to steer current away from the ADCs using this ground fill cut, make sure that it extends to the ground plane layer as well as to the ground fill on the bottom of the board. I think you implied this is what you were going to do in your response, but I just wanted to be sure.

    You also want to make sure you have stitching vias between the ground fill and the ground plane. I did not see them in the image above, but maybe they were just hidden.

    -Bryan

  • 0 in reply to Bryan Lizon86
    Prodigy 180 points

    Hello Bryan,

    thank you for your reply. Yes you interpret my descriptions right. My idea was to have a cut in the ground in all layers to be sure, that the return current flows not through the ADC section. The layout in the picture was just an early design to get an idea. The ground vias you addressed are not in the design, but thats a good idea. In general, would you recommend that idea or would an complete ground plane on all layers (without the cut) the better way?

  • 0 in reply to Tony Steinbock
    TI__Mastermind 35241 points

    Hi Tony,

    Unfortunately I don't have a great answer for your question other than "it depends..."

    If there was minimal current flowing from the switches through the ADC/MCU portion of the board, you might not actually see a benefit from the split. Or, if the current was constant i.e. a relatively fixed value at all times, perhaps this would not cause ground bounce and the split would not help either. But this really depends on your system, and there is no guaranteed correct answer here.

    Moreover, having the split might introduce other unwanted system effects such as more susceptibility to EMI (you can read more about why here: https://e2e.ti.com/support/data-converters/f/data-converters-forum/755516/faq-pcb-layout-guidelines-and-grounding-recommendations-for-high-resolution-adcs)

    That link generally recommends against split ground planes, or ground cuts, in favor of a single solid ground layer. My best recommendation would be to situate the components on your board such that those switches have a clear ground return path that does not intersect the ADC/MCU portion of the board, but I recognize that is likely not an option here. Therefore, I would try the ground plane cut as you have already done, but be prepared to modify the board in case the cut introduces additional issues.

    -Bryan

  • 0 in reply to Bryan Lizon86
    Prodigy 180 points

    Hello Bryan,

    thank you for your reply. The high-side switches control 24V valves. In our application, the valves are switched on, and after a time delay of 3 seconds, we drive the high side switches with a pwm, to reduce the current consumption. As i wrote, each high side switch port takes up to 24V / 0,4A (nominal, without pwm operation). On the same 24V path, which goes to the bottom part of the pcb, there are also two 24V/250mA fans powered, also controlled with pwm. One more point is, that the area size, which goes down, to the 24V consumers is getting a little bit small, because there go several traces from the microcontroller to the switches and fans.

    Thank you for the interesting link. The more I think about it, the more I tend to use a complete ground plane. Here is a larger section of the pcb (still in work). In the marked are you see the two 4-pin connectors for the fans with the circuit parts around. I have to seperate the ground area also in this area, otherwise there is a ground loop around the ADC area. With the ground cut ending in the marked section, i have to go with every signal trace around the ADC section on the left.  To the right of the picture goes also the same ground.

    For your information: the high-side switch is protected againt inductive load by himself and in addition with an diode.

  • 0 in reply to Tony Steinbock
    TI__Mastermind 35241 points

    Thanks for the additional information, Tony.

    It seems like you are moving toward using a solid ground plane. If you have additional questions as you move through the design, please let us know. Also, if you do perform EMI testing, etc.,  and are able to post your results to this thread, that would be helpful for other customers in the future. They may not be able to mimic your system exactly, but at least it would serve as another example when doing their board layout / partitioning.

    -Bryan

  • 0 in reply to Bryan Lizon86
    Prodigy 180 points

    Bryan, thank you for your help! I decide to use a solid ground plane without the cut. In our application, the focus on the ADC is to read in the PT100 values trouble-free. The ADC accuracy is not that critical. We also have other components around the board that can cause EMI interference. So I choose for the first design a solid ground plan for better EMI behavior. 

  • 0 in reply to Tony Steinbock
    TI__Mastermind 35241 points

    Sounds good Tony. I will consider this specific issue resolved for now, but feel free to start a new thread if anything else comes up.

    If you need any help with RTD measurements we have an RTD cookbook that may be useful: https://www.ti.com/lit/an/sbaa275/sbaa275.pdf?ts=1615301905447&ref_url=https%253A%252F%252Fwww.google.com%252F

    We also have linearization firmware for RTDs, thermocouples and thermistors if that is required for your system: https://www.ti.com/tool/ADC-TEMP-SENSOR-FW. Right now this information is specific to the ADS124S08, but you can modify the code to work with any ADC if you are interested.

    As a side note, the ADS124S08 is the next-generation version of the ADS1248. The ADS124S08 has many performance and feature upgrades compared to the ADS1248, and is also offered in a smaller package. You might consider this ADC for future projects.

    -Bryan