Table of Contents
Advertisement
R
Traces
Trace Geometry
For any trace, its characteristic impedance is dependent on its stackup geometry as well as
the trace geometry. In the case of differential traces, the inductive and capacitive coupling
between the tightly coupled pair also determines the characteristic impedance of the
traces.
The impedance of a trace is determined by its inductive and capacitive coupling to nearby
conductors. For example, these conductors can be planes, vias, pads, connectors, and other
traces, including the other closely coupled trace in a differential pair. The substrate
properties, conductor properties, flux linkage area, and distance to a nearby conductor
determine the amount of coupling and hence, the contribution to the final impedance.
2D field solvers are necessary in resolving these complex interactions and contribute to the
calculation of the final impedance of the trace. They are also a useful tool to verify existing
trace geometries.
A common misconception is that two 50Ω single-ended traces can be routed side-by-side
to give a pair with 100Ω differential impedance. While this approximation might be true if
the traces are loosely coupled, routing differential traces in a loosely coupled fashion does
not maximize the noise immunity of differential mode signaling.
Tightly coupled differential pairs are required for all high-speed GTP traces because they
are more sensitive to noise than slower signals. As a general rule of thumb, tight coupling
within a differential pair is achieved by spacing them no more than four trace widths
apart.
Wider traces create a larger cross-sectional area for current to flow and reduce resistive
losses. Use the widest traces that space constraints allow. Because trace width tolerances
are expressed in absolute terms, a wider trace also minimizes the percentage variation of
the manufactured trace, resulting in tighter impedance control along the length of the
transmission line.
Striplines are preferred over microstrips because the reference planes on both sides of the
trace provide radiation shielding. Microstrips are shielded on only one side (by the
reference plane) because they run on the topmost or bottom-most layers, leaving the other
side exposed to the environment.
For best results, the use of a 2D field solver is recommended for verification.
Trace Characteristic Impedance Design
Because the transceivers use differential signaling, the most useful trace configurations are
differential edge-coupled center stripline and differential microstrip. While some
backplanes use the differential broadside-coupled stripline configuration, it is not
recommended for 10 Gb/s operation, because the P and N vias are asymmetrical and
introduce common-mode non-idealities.
With few exceptions, 50Ω characteristic impedance (Z
the channel. In general, when the width/spacing (W/S) ratio is greater than 0.4 (8 mil wide
traces with 20 mil separation), coupling between the P and N signals affects the trace
impedance. In this case, the differential traces must be designed to have an odd mode
impedance (Z
Z
Virtex-5 RocketIO GTP Transceiver User Guide
UG196 (v1.3) May 25, 2007
) of 50Ω , resulting in a differential impedance (Z
0O
= 2 x Z
.
DIFF
0O
www.xilinx.com
) is used for transmission lines in
0
) of 100Ω , because
DIFF
Traces
233
Advertisement
Table of Contents
