SPRACP4A December   2019  – June 2024 AM67 , AM67A , AM68 , AM69 , DRA829J , DRA829V , TDA4AEN-Q1 , TDA4VEN-Q1 , TDA4VH-Q1 , TDA4VM , TDA4VM-Q1

 

  1.   1
  2.   Abstract
  3.   Trademarks
  4. 1Introduction
    1. 1.1 Overview
    2. 1.2 Supporting Documentation
  5. 2High-Speed Interface Design Guidance
    1. 2.1  Trace Impedance
    2. 2.2  Trace Lengths
    3. 2.3  Differential Signal Length Matching
    4. 2.4  Signal Reference Planes
    5. 2.5  Differential Signal Spacing
    6. 2.6  Additional Differential Signal Rules
    7. 2.7  Symmetry in the Differential Pairs
    8. 2.8  Connectors and Receptacles
    9. 2.9  Via Discontinuity Mitigation
    10. 2.10 Back-Drill Via Stubs
    11. 2.11 Via Anti-Pad Diameter
    12. 2.12 Equalize Via Count
    13. 2.13 Surface-Mount Device Pad Discontinuity Mitigation
    14. 2.14 Signal Bending
    15. 2.15 ESD and EMI Considerations
    16. 2.16 ESD and EMI Layout Rules
  6. 3Interface-Specific Design Guidance
    1. 3.1 USB Board Design and Layout Guidelines
      1. 3.1.1 USB Interface Schematic
        1. 3.1.1.1 Support Components
      2. 3.1.2 Routing Specifications
    2. 3.2 DisplayPort Board Design and Layout Guidelines
      1. 3.2.1 DP Interface Schematic
        1. 3.2.1.1 Support Components
      2. 3.2.2 Routing Specifications
    3. 3.3 PCIe Board Design and Layout Guidelines
      1. 3.3.1 PCIe Interface Schematic
        1. 3.3.1.1 Polarity Inversion
        2. 3.3.1.2 Lane Swap
        3. 3.3.1.3 REFCLK Connections
        4. 3.3.1.4 Coupling Capacitors
      2. 3.3.2 Routing Specifications
    4. 3.4 MIPI® D-PHY (CSI2, DSI) Board Design and Layout Guidelines
      1. 3.4.1 CSI-2®, DSI® Interface Schematic
      2. 3.4.2 Routing Specifications
      3. 3.4.3 Frequency-Domain Specification Guidelines
    5. 3.5 UFS Board Design and Layout Guidelines
      1. 3.5.1 UFS Interface Schematic
      2. 3.5.2 Routing Specifications
    6. 3.6 Q/SGMII Board Design and Layout Guidelines
      1. 3.6.1 Q/SGMII Interface Schematic
        1. 3.6.1.1 Coupling Capacitors
      2. 3.6.2 Routing Specifications
  7. 4Board Design Simulations
    1. 4.1 Board Model Extraction
    2. 4.2 Board-Model Validation
    3. 4.3 S-Parameter Inspection
    4. 4.4 Time Domain Reflectometry (TDR) Analysis
    5. 4.5 Simulation Integrity Analysis
      1. 4.5.1 Simulator Settings and Model Usage
      2. 4.5.2 Simulation Parameters
      3. 4.5.3 Simulation Methodology
    6. 4.6 Reviewing Simulation Results
  8. 5References
  9. 6Revision History

2.6 Additional Differential Signal Rules

  • Do not place probe or test points on any high-speed differential signal.
  • Do not route high-speed traces under or near crystals, oscillators, clock signal generators, switching power regulators, mounting holes, magnetic devices, or ICs that use or duplicate clock signals.
  • After BGA breakout, keep high-speed differential signals clear of the SoC because high current transients produced during internal state transitions can be difficult to filter out.
  • When possible, route high-speed differential pair signals on the top or bottom layer of the PCB with an adjacent GND layer. TI does not recommend stripline routing of the high-speed differential signals. (or Stripline routing is recommended for all high-speed SerDes signals in the design. This provides better controlled impedance. Also the signal quality degradation due to EMI is minimized by fabricating traces in between ground planes).
  • Make sure that high-speed differential signals are routed ≥ 90mils from the edge of the reference plane.
  • Make sure that high-speed differential signals are routed at least 1.5W (calculated trace-width × 1.5) away from voids in the reference plane. This rule does not apply where SMD pads on high-speed differential signals are voided.
  • Maintain constant trace width after the SoC BGA escape to avoid impedance mismatches in the transmission lines.
  • Maximize differential pair-to-pair spacing when possible (loosely coupled).