• State Resolved
  • Locked Locked
  • Replies 6 replies
  • Subscribers 47 subscribers
  • Views 936 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.

Question on AFE4490SPO2EVM Schematics

Mohammad Hosseini1
Intellectual 610 points
Other Parts Discussed in Thread: AFE4490, AFE4490SPO2EVM

Hello,

I'm currently designing a reflective pulse oximeter using the AFE4490. I'm trying to use the schematics provided with the AFE4490SPO2EVM as a reference. Please help me understand the following in regards to the schematic on page 46 of the user guide also pictured below. Thanks!

1) What is the purpose of the VCM Shield exactly and its trace on the schematic?

2) What is the purpose of the BAV99W-7-F dual diodes?

3) What does this symbol refer to? Is it related to the vcm shield?

 

4) What is the purpose of the 10 ohm resistors placed between the AFE4490 and MSP430 pins? Are these necessary?

  • 0
    TI__Mastermind 49786 points

    Hello Mohammad,

    1. VCM is a reference voltage that is generated internally and is used to bias the input common mode of the TIA. By shielding the traces of the photodiode connections to the INP and INN inputs with VCM, any leakage current created by the impedance between INP/INN traces and GND line can be prevented.

    2. BAV99W switching diodes are primarily used as diode clamps. If you expect to see accidental higher voltages at the INN, INP, DETP and DETM lines, it is recommended to use clamp diodes to supply and ground to protect the AFE4490. For battery operated systems this might not be necessary.

    3. We used Altium Designer to build the schematics. That symbol is a constraint offered by the tool to impose on the layout. In this case it is to route the INN and INP channels as a differential pair.

    4. The 10 Ohm resistors were placeholders for series termination for signal integrity in case there was ringing on the digital lines. These are not absolutely necessary.

     

    Regards

    Praveen.

  • 0 in reply to Praveen Aroul
    Intellectual 610 points

    Hi Praveen,

    Thanks for the clarifications! Some follow-ups:

    1) So the trace for the VCM shield must literally surround the INP/INN traces as shown in the schematic for the purposes of the PCB?

    2) Is there any minimal specification for the diodes used here? I'm assuming anything with minimal reverse current would be suitable?

    3) I have not used Altium Designer. I'm currently using Eagle for drawing the schematic and later the PCB. Is this something that I need to implement?

  • 0 in reply to Mohammad Hosseini1
    Intellectual 610 points

    Just bumping this up so I can get a response to above follow-up questions. Thanks.

  • 0 in reply to Mohammad Hosseini1
    TI__Mastermind 18285 points

    Mohammad,

    1) Yes, that is correct. For more detail on layout guidelines,refer to the below informaiton.

    Layout Guidelines for INN, INP and VCM signals of AFE44x0

    Route the Receive signals (INN and INP) differentially with tight coupling at approximately the same length. Use VCM signal to shield the INP and INN traces. VCM signal is intended to guard the INN and INP traces from common mode noise (as shown below). VCM is a reference voltage that is generated internally and is used to bias the input common mode of the TIA. By shielding the traces of the photodiode connections to the INP and INN inputs with VCM, any leakage current created by the impedance between INP/INN traces and GND line can be prevented.

    There are no other special guidelines.

     

    Below are few PCB layout tips:

    • Separate Analog and Digital signals
      • The separation of the Analog and Digital section of the PCB keeps noisy digital from the low level analog. However, they must come together at the AFE.
    • AGND and DGND connected at the AFE
      • It is important that the Analog Ground and the Digital Ground be connected together at the AFE. This allows a quick return for the ground currents as the analog and digital portions of the device communicate.
    • Provide good Ground return paths.
      • AGND and DGND are connected at the AFE and also at the power supply, there is a ground loop created. By having a solid ground plane this can be eliminated.

    2) If you don't have any board constraints, you can use the ones we have shown on our schematic. Yes, you want to have minimal reverse current when selecting these.

    3) Which are you referring to. You must implement the layout guidelines and route as a differential pair. And follow specifications for the VCM trace.

    Hope this helps.

  • 0 in reply to Amy Schnoor
    Intellectual 610 points

    Hi Amy, thanks for answering my questions.


    In regards to number 3, I'm not familiar with differential pair routing. This is the first time I'm working on creating my own PCB. In fact, I'm trying to use a breakout board for the AFE4490 in combination with a breadboard and an MCU development board for initial prototyping.


    Can you briefly explain the application of differential pair routing or link me to an explanation?

    Thanks.

  • 0 in reply to Mohammad Hosseini1
    TI__Mastermind 18285 points

    Mohammad,

    Altium's website gives a good definition of differential pair routing. I included the link here for your reference.

    http://techdocs.altium.com/display/ADOH/Differential+Pair+Routing