• State TI Thinks Resolved
  • Locked Locked
  • Replies 19 replies
  • Answers 3 answers
  • Subscribers 15 subscribers
  • Views 1822 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.

ISO7721: Connect GND

Shu-Cheng LIN
Guru 11785 points
Part Number: ISO7721
Other Parts Discussed in Thread: ISO1042

Hi Sirs,

Sorry to bother you.

We would like to know ISO7721
If VCCI and VCCO voltage and GND are the same


Does that still have the effect of isolation protection?

  • 0
    TI__Genius 17100 points

    Hi Shu-Cheng,

    This is no bother! Although the voltages Vcci, Vcco and GNDi, GNDo can be the same voltages connected together, this configuration will not have the effect of isolation.

    In an isolation schematic, GNDi and GNDo should be separate ground planes with no connection to each other. This is also true of Vcci and Vcco: for isolation, they cannot be connected to each other. An example of how this looks on a PCB is shown below:



    Isolation can be achieved in this design! It is a matter of isolating the power supplies and separating the GNDs. Will you like some guidance on how to do this?


    Thank you for posting to E2E,
    Manuel Chavez

  • 0 in reply to Manuel Chavez
    Guru 11785 points

    Hi Sirs,

    Thanks for your reply

    1. As below, our PCB placement will be two ISO1042 on both ends of the board, if the two connectors cannot move,
    How to connect CANH/CANL on both GNDB terminals?

    2. I need to leave 120ohm termination resistor on the path. Why does PCB trace not need impedance control?

  • 0 in reply to Shu-Cheng LIN
    Guru 11785 points

    Hi Sirs,

    Sorry for pushed, have any update on here?

    Thanks!!

  • 0 in reply to Shu-Cheng LIN
    TI__Genius 17100 points

    Hi Shu-Cheng,

    No problem! I apologize for the delay. I have some questions and comments for your points:

    1. Will the two connectors be connected by a cable? If so, both sets of CANH, CANL, and GNDB may be connected through it, however, it is not necessary to connect both GNDB terminals to each other. With or without a cable, there may be a voltage between both GNDB terminals; as long this voltage does not exceed 30V, the the input common mode range will be within recommended conditions
    2. PCB traces have low impedance characteristics compared to cables, so if CAN signals are routed only on PCB, it is priority that CANH and CANL traces are physically as similar as possible (yielding nearly identical trace impedances). When using cables, termination resistors are used to minimize reflections, but this is not necessary if signals are only routed on PCBs - how is your termination resistor connected? If it is left populated, input signals might be slightly attenuated.

    I hope this is a helpful response! Please do reply with any additional questions or concerns.


    Thank you for your time,
    Manuel Chavez

  • 0 in reply to Manuel Chavez
    Guru 11785 points

    Hi Sirs,

    Thanks for your reply.

    At present, our termination resistors are expected to be implemented in the following two locations.
    Please help me to confirm if there is any problem? thanks

  • 0 in reply to Shu-Cheng LIN
    Guru 11785 points

    Hi Sirs,

    Any update on here?

    One more question, if the VCC2 5V power source is independently supplied, the GND of ISO1042 is connected to ISO GND.
    Is the GND of the power IC supplied to VCC2 also need connected to ISO GND?

  • 0 in reply to Shu-Cheng LIN
    Guru 11785 points

    Hi Sirs,

    Update our board schematic as below

    This board is the red part of the system block, could you help double check it? Any suggestion are welcome 

    Schematic:

    system block

    BCB Board  Block Diagram 

  • 0 in reply to Shu-Cheng LIN
    Guru 11785 points

    Hi Sirs,

    Sorry for pushed, have any update on this topic?

    Thanks!!

  • 0 in reply to Shu-Cheng LIN
    Guru 11785 points

    Hi Sirs,

    Sorry for pushed, have any update on this topic?

    Any suggest are welcome.

    Thanks!!

  • 0 in reply to Shu-Cheng LIN
    TI__Genius 17100 points

    Hi Shu-Cheng,

    I apologize for the delay in my responses.

    Regarding the post with termination resistors on June 14th, the location of these termination resistors is good if the LED Driver and BCM nodes are the longest nodes in the network. It seems like they are, but if the ATX 12 board has more cable than one of the other two nodes, the termination resistors should be in different places.

    On the following question, both Digital Ground and ISO Ground are set up correctly. Only what is on the right side of the isolation barrier (which you have in the red box) should be connected to ISO Ground.

    Thank you for including the block diagram! In the 55.pdf schematic, it will be beneficial to include a 10uF capacitor on pin 2 of the transformer (U32). Capacitors C304 - C307 are not critical, but of course you may leave these in.


    I appreciate your patience with this response; please feel free to follow up with additional concerns of comments.


    Thank you for your time,
    Manuel Chavez

  • 0 in reply to Manuel Chavez
    Guru 11785 points

    Hi Sirs,

    Thanks for your reply.

    About the 55.pdf schematic review, in addition to U32.Pin2 need to add a 10uF capacitor, others schematic looks good. Is it correct?

  • 0 in reply to Shu-Cheng LIN
    TI__Genius 17100 points

    Hi Shu-Cheng,

    Yes, the schematic from what is shown looks to be properly connected. As an additional note, please do ensure that the 3V3 and 4V0 power supplies are isolated from GND_ISO.

    Are there additional questions I can help with?


    Respectfully,
    Manuel Chavez

  • 0 in reply to Manuel Chavez
    Guru 11785 points

    Hi Sirs,

    Thanks for your reply.

    One more question, 

    We wonder if we need to do the impedance control and twist pair for the CAN Bus pair signals (CANH/CANL) on the interconnection cables?

    Could you help to clarify? Thank!!

  • 0 in reply to Shu-Cheng LIN
    TI__Genius 17100 points

    Hi Shu-Cheng,

    Yes, feel free to use twisted pair for the CAN bus pair signals. The cables should have a nominal impedance of 120 Ohms to minimize reflections. Ensure you are minimizing cable lengths for stubs, which is what the cable for the ATX 12 board will be.

    Can you please share the part numbers of C304 - C307 capacitors? I have looked for them inline without any results so far.


    Thank you for your time,
    Manuel Chavez

  • 0 in reply to Manuel Chavez
    Guru 11785 points

    Hi Sirs,

    Thanks for your reply.

    Regarding the ISO7721 dual-channel digital Isolators,

    Due to design rule reminder keep the space free under the component,

    Could you please help to check how many width for the clearing area?

    We wonder to know the minimum width for the design rule, thanks a lot.

  • 0 in reply to Shu-Cheng LIN
    TI__Genius 17100 points

    Hi Shu-Cheng,

    The isolation barrier width in the PCB can be set using the width between the isolated and non-isolated pads of the device. The minimum width varies with package, and for highest creepage and clearance use the widest land pattern possible. Reference land patterns are shown in pages 30 and 33 of the ISO7721 datasheet

    For an ISO7721 in a D package, 3.85mm and 4.1mm widths of the isolation barrier are shown below:



    and for an ISO7721 in a DW package, the width parameters are greater:




    Is this the dimension you are looking for? Please let me know!


    Thank you for your time,
    Manuel Chavez

  • 0 in reply to Manuel Chavez
    Guru 11785 points

    Hi Sirs,

    Thanks for your reply.

    We wonder if the CAN Bus can use the 100 ohm impedance control for cable instead of 120 ohm

    since the 120 ohm impedance is not as common as 100 ohm impedance for cable vendors.

  • 0 in reply to Manuel Chavez
    Guru 11785 points

    Hi Sirs,

    Thanks for your reply.

    Due to the ISO7721 have different reference GND,

    Could you please help to confirm the minimum GND moat distance?

     

    For example, due to we used the ISO7721FDR for the SOIC-8 D package,

    The SOIC-8 widths is 3.85 mm, Does it meet the GND ISO moat need 3.85 mm?

    Because the 3.85mm is too wide for layout design, Does it possible to reduce the width to meet design rule?

  • 0 in reply to Shu-Cheng LIN
    TI__Genius 17100 points

    Hi Shu-Cheng,

    Since the CAN standard is defined with 120 Ohm impedance cable, if 100 Ohm cable is used, it will not technically be CAN standard compliant. From a device functionality perspective, 100 Ohm cable can be used, and if you choose to use it, the termination resistor should match the cable impedance of 100 Ohm.

    Regarding the ISO7721FDR, the isolation barrier or "moat" distance directly affects isolation rating. By reducing the thickness of the moat, please know that the creepage/clearance and therefore isolation voltage rating will decrease if there are exposed traces, pads, or device pins closer than the device's own creepage and clearance distance of 4mm


    Thank you for your time,
    Manuel Chavez