SPRAD66B February   2023  – December 2024 AM62A3 , AM62A3-Q1 , AM62A7 , AM62A7-Q1 , AM62D-Q1 , AM62P , AM62P-Q1

 

  1.   1
  2.    AM62Ax, AM62Px, AM62Dx LPDDR4 Board Design and Layout Guidelines
  3.   Trademarks
  4. 1Overview
    1. 1.1 Board Designs Supported
    2. 1.2 General Board Layout Guidelines
    3. 1.3 PCB Stack-Up
    4. 1.4 Bypass Capacitors
      1. 1.4.1 Bulk Bypass Capacitors
      2. 1.4.2 High-Speed Bypass Capacitors
    5. 1.5 Velocity Compensation
  5. 2LPDDR4 Board Design and Layout Guidance
    1. 2.1  LPDDR4 Introduction
    2. 2.2  LPDDR4 Device Implementations Supported
    3. 2.3  LPDDR4 Interface Schematics
    4. 2.4  Compatible JEDEC LPDDR4 Devices
    5. 2.5  Placement
    6. 2.6  LPDDR4 Keepout Region
    7. 2.7  Net Classes
    8. 2.8  LPDDR4 Signal Termination
    9. 2.9  LPDDR4 VREF Routing
    10. 2.10 LPDDR4 VTT
    11. 2.11 CK and ADDR_CTRL Topologies
    12. 2.12 Data Group Topologies
    13. 2.13 CK0 and ADDR_CTRL Routing Specification
    14. 2.14 Data Group Routing Specification
    15. 2.15 Channel, Byte, and Bit Swapping
    16. 2.16 Data Bus Inversion
  6. 3LPDDR4 Board Design Simulations
    1. 3.1 Board Model Extraction
    2. 3.2 Board-Model Validation
    3. 3.3 S-Parameter Inspection
    4. 3.4 Time Domain Reflectometry (TDR) Analysis
    5. 3.5 System Level Simulation
      1. 3.5.1 Simulation Setup
      2. 3.5.2 Simulation Parameters
      3. 3.5.3 Simulation Targets
        1. 3.5.3.1 Eye Quality
        2. 3.5.3.2 Delay Report
        3. 3.5.3.3 Mask Report
    6. 3.6 Design Example
      1. 3.6.1 Stack-Up
      2. 3.6.2 Routing
      3. 3.6.3 Model Verification
      4. 3.6.4 Simulation Results
  7. 4Additional Information: SOC Package Delays
  8. 5Summary
  9. 6References
  10. 7Revision History

1.2 General Board Layout Guidelines

To verify good signaling performance, the following general board design guidelines must be followed:

  • Always follow TI's example layouts and EVM designs as close as possible. If concepts or routing strategies are not understood, then ask questions on E2E.
  • All signals need ground reference (strongly suggest on both sides).
  • Avoid crossing plane splits in the signal reference planes.
  • Use the widest trace that is practical between decoupling capacitors and memory modules.
  • Minimize inter-symbol interference (ISI) by keeping impedances matched. This is especially true for any T-branch signals where trace widths are adjusted to match trace impedance.
  • Minimize crosstalk by isolating sensitive signals, such as strobes and clocks, and by using a proper PCB stack-up.
  • Avoid return path discontinuities by adding vias or capacitors whenever signals change layers and reference planes.
  • Minimize reference voltage noise through proper isolation and proper use of decoupling capacitors on the reference input pins on the SDRAMs.
  • Keep the signal routing stub lengths as short as possible.
  • Add additional spacing for clock and strobe nets to minimize crosstalk.
  • Maintain a common ground (also called VSS) reference for all signals and for all bypass and decoupling capacitors.
  • Consider the differences in propagation delays between microstrip and stripline nets when evaluating timing constraints.
  • Via-to-via coupling can be significant part of PCB-level crosstalk. Dimension and pitch of vias is important. For high speed interfaces, consider GND shielding vias. This via coupling is one factor for recommending data signals be routed on layers closest to processor.
  • Via stubs affect signal integrity. Via back-drilling can improve signal integrity, and is required in some instances.

For more information, see the High-Speed Interface Layout Guidelines application note. This provides additional general guidance for successful routing of high-speed signals.