• State Resolved
  • Replies 2 replies
  • Subscribers 34 subscribers
  • Views 72 views
  • Users 0 members are here
Support feedback
Options
Options
Related

TCAN1044A-Q1: 120 ohm CAN differential PCB impedance

Francisco Vera
Prodigy 180 points

Part Number: TCAN1044A-Q1

Hello,

I am designing a CAN interface using the TCAN1044A-Q1 and I would like to ask for your recommendation regarding the PCB trace impedance.

My PCB stack-up makes it difficult to achieve a 120 ohm differential impedance without using very narrow traces. The relevant geometry is:

  • Internal CANH/CANL differential pair

  • Trace width: 0.10 mm

  • Differential spacing: 0.34 mm

  • Copper thickness: 18 µm

  • H1 to the GND reference plane: 0.10 mm

  • H2 to the adjacent layer: 0.36 mm

  • Dielectric Dk: approximately 4.45 @ 100 MHz

With this geometry, my field-solver calculation gives approximately 100 ohm differential impedance, compared with the nominal 120 ohm CAN bus impedance, so there is approximately a 17–20% impedance deviation.

The CANH/CANL routing from the TCAN1044A-Q1 to the CAN connector is approximately 90 mm.

This limitation is caused by the fact that the same PCB stack-up is also being used for high-speed USB and Ethernet interfaces, which impose specific controlled-impedance requirements that must be met. Therefore, the available trace geometry for the CAN differential pair is constrained by the overall PCB stack-up and the impedance requirements of these other interfaces.

My main question is:

Would a 100 ohm differential PCB impedance, rather than 120 ohm, be a significant concern for a 90 mm CANH/CANL connection to the TCAN1044A-Q1?

I am particularly interested in whether the 20% impedance deviation is likely to cause a meaningful signal-integrity issue for this PCB trace length, or whether the relatively short 90 mm section can reasonably be treated as a small impedance discontinuity compared with the 120 ohm CAN cable.

If 120 ohm should be considered necessary in this case, could you recommend how you would approach this problem? I would prefer to avoid reducing the trace width further because the transceiver has a 130 mA bus-fault current, and I would like to maintain adequate PCB trace robustness.

Thank you in advance for your advice.

  • +1
    TI__Guru* 80202 points

    Hi Francisco,

    Please note that a 120 Ω differential impedance is preferred for the CANH / CANL PCB routing because it minimizes the impedance discontinuity between the PCB and the typical 120 Ω CAN bus. However, it is not necessarily mandatory for a short PCB segment. I.e., per the proposed ~ 90 mm CANH / CANL routing, a calculated differential impedance of approximately 100 Ω represents a relatively short impedance discontinuity and is unlikely by itself to cause a significant signalintegrity issue, particularly at lower CAN data rates.

    Given the PCB stack-up constraints and the need to maintain adequate trace width for manufacturing and robustness, I would not recommend reducing the trace width solely to achieve exactly 120 Ω. Instead, maintain a symmetrical CANH / CANL pair with a continuous reference plane, minimize stubs / vias, and keep the routing as short as practical, especially for 5 Mbps or higher to help confirm any adequate signal-integrity margin, thanks.

    Best Regards,

    Michael.

  • 0 in reply to Michael Ikwuyum
    Prodigy 180 points

    Hi Michael,

    Thank you very much for the detailed explanation and recommendation.

    In my particular case, the maximum CAN data rate is limited to 1 Mbps, so based on your guidance, I understand that the approximately 100 Ω differential impedance over the ~90 mm CANH/CANL routing should not be a significant concern.

    I will therefore keep the current trace width and geometry rather than reducing the width just to achieve exactly 120 Ω, while following your recommendations regarding symmetrical routing, continuous GND reference, and minimizing stubs and vias.

    Thanks again for your help.

    Best regards,
    Francisco