Intel Agilex® 7 Device Family High-Speed Serial Interface Signal Integrity Design Guidelines

ID 683864
Date 6/15/2023
Document Table of Contents PCB Vias

  • Vias impact high-speed channel loss and the timing budget, so use as few vias as possible for the high-speed differential channel.
  • Keep impedance continuity between the high-speed PCB via and trace. Vias usually have higher capacitance and lower impedance than traces.
  • Optimize via impedance, using a 3D electromagnetic (EM) field solver, by sweeping the anti-pad width, length, and radius for your specific stackup, drill size, and via stub. Keep in mind that:
    • The smaller the drill size, the higher the via impedance
    • The larger the anti-pad size, the higher the via impedance
    • The shorter the via stub, the higher the via impedance
    • The smaller the via top, bottom, and functional pads, the higher the via impedance
Figure 11. Hex Pattern BGA Via Optimization
  • Make sure that each high-speed signal via has a ground via for reference, and make sure that the two signal vias of a differential pair have symmetrical ground vias as the above figure shows. If you do not do this, mode conversion is introduced.
  • Remove non-functional pads for high-speed signal vias and ground vias to lower via capacitance.
  • Make the closest TX and RX signal via coupling length as short as possible through an appropriate layer assignment.
Figure 12. Via Coupling Reduction by Routing Layer Assignment (18L Example)
  • During insertion loss evaluation, a resonance can occur in the frequency range of three times the Nyquist frequency. Control the via stub length to avoid this resonance.