DRA722_17 Datasheet, PDF (367/408 Pages) Texas Instruments – Infotainment Applications Processor

www.ti.com
DRA722, DRA724, DRA725, DRA726
SPRS956B – MARCH 2016 – REVISED JANUARY 2017
8.5.4.2 TMDS General Routing Guidelines
The TMDS signals are high speed differential pairs. Care must be taken in the PCB layout of these signals
to ensure good signal integrity.
The TMDS differential signal traces must be routed to achieve 100 Ohms (+/- 10%) differential impedance
and 60 ohms (+/-10%) single ended impedance. Single ended impedance control is required because
differential signals can’t be closely coupled on PCBs and therefore single ended impedance becomes
important.
These impedances are impacted by trace width, trace spacing, distance to reference planes, and dielectric
material. Verify with a PCB design tool that the trace geometry for both data signal pairs results in as
close to 60 ohms impedance traces as possible. For best accuracy, work with your PCB fabricator to
ensure this impedance is met.
In general, closely coupled differential signal traces are not an advantage on PCBs. When differential
signals are closely coupled, tight spacing and width control is necessary. Very small width and spacing
variations affect impedance dramatically, so tight impedance control can be more problematic to maintain
in production.
Loosely coupled PCB differential signals make impedance control much easier. Wider traces and spacing
make obstacle avoidance easier, and trace width variations don’t affect impedance as much, therefore it’s
easier to maintain accurate impedance over the length of the signal. The wider traces also show reduced
skin effect and therefore often result in better signal integrity.
Some general routing guidelines regarding TMDS:
• Avoid crossing splits reference plane(s).
• Shorter trace length is preferred.
• Distance between common mode filter (CMF) and ESD protection device should be as short as
possible
• Distance between ESD protection device and HDMI connector should be as short as possible.
Table 8-13 shows the routing specifications for the TMDS signals.
Table 8-13. TMDS Routing Specifications
PARAMETER
MIN
TYP
MAX
UNIT
Device balls to HDMI header trace length
4000
Mils
Skew within a differential pair
3
5
Mils
Number of stubs allowed on TMDS traces
0
stubs
TMDS pair differential impedance
90
100
110
Ω
TMDS single-ended impedance
54
60
66
Ω
Number of vias on each TMDS trace
0
Vias
TMDS differential pair to any other trace spacing^{(1) (2) (3)}
2×DS
3xDS
Mils
Number of ground plane cuts allowed within HDMI routing region (except for specific
ground carving as explained in this document)
0
Cuts
Number of layers between HDMI routing region and reference ground plane
0
Layers
PCB trace width
4.4
Mils
(1) DS = differential spacing of the traces.
(2) Exceptions may be necessary in the SoC package BGA area.
(3) GND guard-bands may be closer, but should not be allowed to affect the impedance of the differential pair routing. GND guard-bands to
isolate HDMI differential pairs from all other signals is recommended.
Item
ESD part number
Table 8-14. TDMS Routing Recommendations
Description
TPD1E05U06
Reason
Minimize capacitance (0.42pF)
Copyright © 2016–2017, Texas Instruments Incorporated
Applications, Implementation, and Layout 367
Submit Documentation Feedback
Product Folder Links: DRA722 DRA724 DRA725 DRA726