RH56D-PCI Ver la hoja de datos (PDF) - Unspecified

Número de pieza

componentes Descripción

Fabricante

RH56D-PCI

Host-Controlled V.90/K56flex™ Modem device Family for Desktop Applications

Unspecified 

RH56D-PCI Modem Designer’s Guide

4.2.2 Placement of Modem Devices

1. Rotate and position the Modem devices to minimize the number of vias on all traces.

2. Rotate and position the device with the PCI interface to minimize trace lengths of PCI signals.

3. Rotate and position the device with the analog interface the analog section is separated from the PCI area and other fast

signals.

4.2.3 Trace Routing and Length on PCI Signals

1. The modem device pinouts are arranged such that signal routing to the PCI connector can be done with at most one via.

If any signals cross, the net-list is wrong. The essential rules are: consistent trace aperture, minimum number of vias,

trace bends at 45 degree angle maximum.

2. Provide 15 mils minimum trace widths for the PCICLK, MRXCLK, MTXCLK, MPLLOUT, BIT_CLK clock signals. Keep the

trace widths as consistent as possible to minimize impedance changes. This also means that the trace going into a

series terminating resistor should the same on both sides. No vias are permitted on the clock-carrying traces. Clocks

should always be routed on one side of the board.

3. PCI 2.1 specification puts a strict length limit on PCI signals. The PCICLK trace must be 2.5 ± 0.1" in length; other PCI

signal traces should be less than 1.5" in length. Conexant reference designs achieve the required length by performing a

zigzag routing with (a) rounded corners for lower EMI and (b) approximately double width traces compared to other PCI

interface signals for lower impedance/EMI.

4. The PCICLK signal is one of the largest sources of EMI on PCI peripheral designs. Surround this trace on both sides by

guard-bands of digital ground that envelope PCICLK along the entire length. This technique also aims at approximating

the required impedance relationship of PCICLK with respect to ground distribution. Connect this guard-band to ground

pins immediately next to the PCICLK pin at the PCI connector. . Also, see Section 4.1.3.

5. Provide guard-band also for the OSC_OUT clock trace. Decouple guard-band with a surface mount capacitors.

4.2.4 Grounding

Because EMI always takes the easiest path to earth ground, ensure that EMI has no problem finding it in a harmless way.

1. Provide ground paths to the bracket. The best ground is provided by the bracket, not by the ground pins on the bus

(while the ground pins provide effective signal returns to the motherboard, at high frequencies these traces become

inductors that acquire higher impedance with increasing frequency). The bracket ground which connects to the chassis is

quite beneficial in dealing with unwanted EMI. This includes using both bracket screws with as much contact surface

area as possible to ground (including under the screw head), and pin 1 on any audio connectors (which tie to the bracket

via the connector chassis and screw). On the bracket edge of the board, place a ground strip on both sides of the board.

The bracket ground (chassis ground) depends on the PC’s case, so choose a system for FCC testing with good EMI

shielding. Experience has shown different PC brands can have quite different EMI characteristics of their own.

2. Surround noisy signals, especially clocks, with a guard-band of thick traces of ground. Pay special attention to where the

guard-bands are grounded, as the effectiveness of this technique will be greatly diminished with the increased physical

distance.

3. When vias must be used on traces with power/ground distribution, use multiple vias rather than a single via. The more

vias, the lower the impedance.

4. Avoid vias on traces carrying fast signals at any cost. Every place the impedance on a trace changes an additional EMI

is generated. RipTide device signals are designed to route to the PCI connector and codec without signal crossover.

Therefore, there should be very little need for vias. PCI signals on the blank side of the board should have only one via.

Other PCI signals should have no vias.

5. If radiated emissions move 6 or more dBuV just by slightly moving connected cables, the grounding technique used in

design should be improved. At this point, maximize dumping EMI energy directly to the bracket ground without dumping

too much EMI energy to scattered ground traces on the board.

4.2.5 Filtering

1. A general rule of thumb is to filter every connector on the board. On audio combo boards, these filters take the form of

ferrite beads and capacitors. Place a ferrite in series with the signal and a capacitor between the signal and ground. After

the signal is filtered, it must not be exposed to any board noise. Therefore, the filter must be as close to the connector as

possible and filtered signals kept away from the digital ground and power.

4-6

Conexant

1213

Conexant Proprietary Information

Share Link: