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

Download PDF
ID 683864
Date 11/20/2024
Public
Document Table of Contents
Document Table of Contents x
1. Signal Integrity (SI) in High-Speed PCB Designs
1. Signal Integrity (SI) in High-Speed PCB Designs x
1.1. Supported Protocols 1.2. Channel Insertion Loss (IL) Budget Calculation 1.3. PCB Materials and Stackup Design Guidelines 1.4. PCB Design Guidelines 1.5. Document Revision History for the Agilex™ 7 Device Family High-Speed Serial Interface Signal Integrity Design Guidelines
1.3. PCB Materials and Stackup Design Guidelines x
1.3.1. Mitigating Insertion Loss with Dielectric Material 1.3.2. Power Layers 1.3.3. Reference Planes 1.3.4. Layer Assignment 1.3.5. Impedance 1.3.6. Via Drill Size 1.3.7. Fiber Weave 1.3.8. Reference Stackup
1.4. PCB Design Guidelines x
1.4.1. General PCB Design Guidelines 1.4.2. E-Tile PCB Design Guidelines 1.4.3. F-Tile PCB Design Guidelines 1.4.4. P-Tile PCB Design Guidelines 1.4.5. R-Tile PCB Guidelines
1.4.1. General PCB Design Guidelines x
1.4.1.1. PCB Traces 1.4.1.2. PCB Vias 1.4.1.3. Connector Breakout 1.4.1.4. AC Coupling Capacitor 1.4.1.5. Others
1.4.3. F-Tile PCB Design Guidelines x
1.4.3.1. F-Tile Features and Capabilities 1.4.3.2. Optimizing the Passive Channel 1.4.3.3. COM Simulations 1.4.3.4. Simulating the Active Channel
1.4.5. R-Tile PCB Guidelines x
1.4.5.1. R-Tiles Features and Capabilities 1.4.5.2. R-Tile Design Layout Examples 1.4.5.3. Landing Pad Cut-out Optimization of AC Coupling Capacitor 1.4.5.4. R-tile HSSI Breakout Routing in BGA Area and MCIO connector Pin Area 1.4.5.5. AC Coupling Capacitor Placement Around MCIO Connector 1.4.5.6. PCIe Gen5 Add-in Card Edge Finger Breakout Design Guidelines
1. Signal Integrity (SI) in High-Speed PCB Designs

1.4.1.2. PCB Vias

  • Via transitions impact high-speed channel loss and the timing budget, so use as few transitions via as possible for the high-speed differential channel.
  • For deep signal vias, the top and bottom ends usually show lower impedance while the middle segments show higher impedance.
  • 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. An oval or circular anti-pad can be considered for via optimization. The following figure shows an oval anti-pad for a Hex pattern. 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. The ground vias need to connect to at least the lower reference ground plane of the signal routing.
  • 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.
Level Two Title