ADV3003

Rev. 0 | Page 13 of 16

The ADV3003 buffers the TMDS signals; therefore, the input

traces can be considered electrically independent of the output

traces. In most applications, the quality of the signal on the input

TMDS traces is more sensitive to the PCB layout. Regardless of

the data being carried on a specific TMDS channel, or whether

the TMDS line is at the input or the output of the ADV3003, all

four high speed signals should be routed on a PCB in accordance

with the same RF layout guidelines.

Layout for the TMDS Signals

The TMDS differential pairs can either be microstrip traces,

routed on the outer layer of a board, or stripline traces, routed

on an internal layer of the board. If microstrip traces are used,

there should be a continuous reference plane on the PCB layer

directly below the traces. If stripline traces are used, they must

be sandwiched between two continuous reference planes in the

PCB stack-up. Additionally, the p and n of each differential pair

must have a controlled differential impedance of 100 Ω. The

characteristic impedance of a differential pair is a function of

several variables including the trace width, the distance separating

the two traces, the spacing between the traces and the reference

plane, and the dielectric constant of the PC board binder material.

Interlayer vias introduce impedance discontinuities that can

cause reflections and jitter on the signal path; therefore, it is

preferable to route the TMDS lines exclusively on one layer of the

board, particularly for the input traces. In addition, to prevent

unwanted signal coupling and interference, route the TMDS

signals away from other signals and noise sources on the PCB.

Both traces of a given differential pair must be equal in length

to minimize intrapair skew. Maintaining the physical symmetry

of a differential pair is integral to ensuring its signal integrity;

excessive intrapair skew can introduce jitter through duty cycle

distortion (DCD). The p and n of a given differential pair should

always be routed together to establish the required 100 Ω

differential impedance. Enough space should be left between

the differential pairs of a given group so that the n of one pair

does not couple to the p of another pair. For example, one tech-

nique is to make the interpair distance 4× to 10× wider than the

intrapair spacing.

Any group of four TMDS channels (input or output) should

have closely matched trace lengths to minimize interpair skew.

Severe interpair skew can cause the data on the four different

channels of a group to arrive out of alignment with one another.

A good practice is to match the trace lengths for a given group

of four channels to within 0.05 inches on FR4 material.

The length of the TMDS traces should be minimized to

reduce overall signal degradation. Commonly used PC board

material such as FR4 is lossy at high frequencies, so long traces

on the circuit board increase signal attenuation, resulting in

decreased signal swing and increased jitter through intersymbol

interference (ISI).

Controlling the Characteristic Impedance of a TMDS

Differential Pair

The characteristic impedance of a differential pair depends on

a number of variables including the trace width, the distance

between the two traces, the height of the dielectric material

between the trace and the reference plane below it, and the

dielectric constant of the PCB binder material. To a lesser

extent, the characteristic impedance also depends upon the

trace thickness and the presence of solder mask.

Many combinations can produce the correct characteristic imped-

ance. It is generally required to work with the PC board fabri-

cator to obtain a set of parameters to produce the desired results.

One consideration is how to guarantee a differential pair with a

differential impedance of 100 Ω over the entire length of the

trace. One technique to accomplish this is to change the width

of the traces in a differential pair based on how closely one trace

is coupled to the other. When the two traces of a differential

pair are close and strongly coupled, they should have a width

that produces a 100 Ω differential impedance. When the traces

split apart, for example, to go into a connector, and are no

longer so strongly coupled, the width of the traces should be

increased to yield a differential impedance of 100 Ω in the new

configuration.

Ground Current Return

In some applications, it may be necessary to invert the output

pin order of the ADV3003. This requires routing of the TMDS

traces on multiple layers of the PCB. When routing differential

pairs on multiple layers, it is also necessary to reroute the corres-

ponding reference plane to provide one continuous ground

current return path for the differential signals. Standard plated

through-hole vias are acceptable for both the TMDS traces and

the reference plane. An example of this routing is illustrated in

Figure 27. To lower the impedance between the two ground

planes, additional through-hole vias should be used to stitch the

planes together, as space allows.

PCB DIELECTRIC

SILKSCREEN

SILKSCREEN

PCB DIELECTRIC

PCB DIELECTRIC

LAYER 2: GND (REFERENCE PLANE)

LAYER 4: SIGNAL (MICROSTRIP)

THROUGH-HOLE VIAS

LAYER 1: SIGNAL (MICROSTRIP)

KEEP REFERENCE PLANE

ADJACENT TO SIGNAL ON ALL

LAYERS TO PROVIDE CONTINUOUS

GROUND CURRENT RETURN PATH.

LAYER 3: PWR

(REFERENCE PLANE)

Figure 27. Example Routing of Reference Plane