AN 672: Transceiver Link Design Guidelines for High-Gbps Data Rate Transmission

Download PDF
ID 683624
Date 1/29/2020
Public
Document Table of Contents
Document Table of Contents x
1. AN 672: Transceiver Link Design Guidelines for High-Gbps Data Rate Transmission
1. AN 672: Transceiver Link Design Guidelines for High-Gbps Data Rate Transmission x
1.1. PCB Material Selection 1.2. Stackup Design 1.3. Channel Design 1.4. Summary 1.5. Document Revision History for the AN 672: Transceiver Link Design Guidelines for High-Gbps Data Rate Transmission
1.1. PCB Material Selection x
1.1.1. Loss Tangent and Dissipation Factor 1.1.2. Dielectric Constant 1.1.3. Fiberglass Weave 1.1.4. Copper Surface Roughness
1.3. Channel Design x
1.3.1. BGA Channel Breakout 1.3.2. Channel Routing Design 1.3.3. Edge Coupling 1.3.4. Broadside Coupling 1.3.5. Transparent Via Design 1.3.6. Blocking Cap Optimization 1.3.7. Connectors Optimization
1.3.2. Channel Routing Design x
1.3.2.1. Trace Width Selection 1.3.2.2. Loose vs. Tight Coupled Traces 1.3.2.3. Crosstalk Control
1.4. Summary x
1.4.1. PCB Material Selection 1.4.2. Stackup Design 1.4.3. Channel Design 1.4.4. References
1. AN 672: Transceiver Link Design Guidelines for High-Gbps Data Rate Transmission

1.2. Stackup Design

The assignment of critical high-speed routing layers within the PCB stack-up is a critical part of the design decision. The assignment of high-speed signal layers within the stackup directly affects the signal performance. Signals routed on external layers of the PCB board are referred to as microstrip, while those routed on internal layers are called stripline.

Figure 9.  Differential Microstrip vs. Stripline Construction

Differential Microstrip vs. Stripline Construction

By manipulating the various parameters such as trace width (W), separation (S), and height from the reference plane (H for microstrip and H1, H2 for stripline), the trace impedance can be adjusted appropriately. Additionally, edge-coupled crosstalk from neighboring traces can be well-controlled by adjusting the pair separation (D). For more information on crosstalk, refer to Crosstalk Control.

Table 2.  Microstrip vs. Stripline
Topology Advantages Disadvantages
Microstrip
  • Thinner dielectric for 100-Ω traces
  • No via for top routing
  • No via stubs for bottom routing
  • Only 2 routing layers possible
  • Higher EMI radiation
  • Both near-end crosstalk (NEXT) and far-end crosstalk (FEXT) concerns
Stripline
  • Many routing layers possible
  • Inherent EMI shielding surrounding layers
  • No FEXT concerns
  • Thicker dielectric required for 100 Ω
  • NEXT concerns
  • Via must be used
  • Via stubs require back-drilling

The decision to use one topology over the other examines the first-order factors that affect signal bandwidth. While impedance and crosstalk can be well-controlled in both routing topologies, stripline provides lower signal attenuation vs. microstrip for the same trace width and copper thickness.

Figure 10. Stripline vs. Microstrip Insertion Loss (Sdd21)

Stripline vs. Microstrip Attenuation

Figure 11. Stackup Construction

Stackup Construction

Note: For the same trace width and copper thickness considerations, stripline results in less signal attenuation compared with microstrip.
Related Information
Level Two Title