Thursday, September 11, 2008

USB 2.0 Board Design and Layout Guidelines

Clock frequencies generate the main source of energy in a USB design. The USB differential DP/DM pairs operate in high-speed mode at 480 Mbps. System clocks can operate at 12 MHz, 48 MHz, and 60 MHz. The USB cable can behave as a monopole antenna; take care to prevent RF currents from coupling onto the cable.

When designing a USB board, the signals of most interest are:

  1. Device interface signals: Clocks and other signal/data lines that run between devices on the PCB.
  2. Power going into and out of the cable: The USB connector socket pin 1 (VBUS ) may be heavily filtered and need only pass low frequency signals of less than ~100 KHz. The USB socket pin 4 (analog ground) must be able to return the current during data transmission, and must be filtered sparingly.
  3. Differential twisted pair signals going out on cable, DP and DM: Depending upon the data transfer rate, these device terminals can have signals with fundamental frequencies of 240 MHz (high speed), 6 MHz (full speed), and 750 kHz (low speed).
  4. External crystal circuit (device terminals XI and X0): 12 MHz, 19.2 MHz, 24 MHz, and 48 MHz fundamental. When using an external crystal as a reference clock, a 24 MHz and higher crystal is highly recommended.
General Routing and Placement

Use the following routing and placement guidelines when laying out a new design for the USB physical layer (PHY). These guidelines help minimize signal quality and electromagnetic interference (EMI) problems on a four-or-more layer evaluation module (EVM).

  1. Place the USB PHY and major components on the un-routed board first.
  2. Route the high-speed clock and high-speed USB differential signals with minimum trace lengths.
  3. Route the high-speed USB signals on the plane closest to the ground plane, whenever possible.
  4. Route the high-speed USB signals using a minimum of vias and corners. This reduces signal reflections and impedance changes.
  5. When it becomes necessary to turn 90°, use two 45° turns or an arc instead of making a single 90° turn. This reduces reflections on the signal traces by minimizing impedance discontinuities.
  6. Do not route USB traces under or near crystals, oscillators, clock signal generators, switching regulators, mounting holes, magnetic devices or IC’s that use or duplicate clock signals.
  7. Avoid stubs on the high-speed USB signals because they cause signal reflections. If a stub is unavoidable, then the stub should be less than 200 mils.
  8. Route all high-speed USB signal traces over continuous planes (VCC or GND), with no interruptions. Avoid crossing over anti-etch, commonly found with plane splits.
Board Stackup
Because of the high frequencies associated with the USB, a printed circuit board with at least four layers is recommended; two signal layers separated by a ground and power layer as shown below:

The majority of signal traces should run on a single layer, preferably SIGNAL1. Immediately next to this layer should be the GND plane, which is solid with no cuts. Avoid running signal traces across a split in the ground or power plane. When running across split planes is unavoidable, sufficient decoupling must be used. Minimizing the number of signal vias reduces EMI by reducing inductance at high frequencies.

Cable Connector Socket

Short the cable connector sockets directly to a small chassis ground plane (GND strap) that exists immediately underneath the connector sockets. This shorts EMI (and ESD) directly to the chassis ground before it gets onto the USB cable. This etch plane should be as large as possible, but all the conductors coming off connector pins 1 through 6 must have the board signal GND plane run under. If needed, scoop out the chassis GND strap etch to allow for the signal ground to extend under the connector pins. Note that the etches coming from pins 1 and 4 (VBUS power and GND) should be wide and via-ed to their respective planes as soon as possible, respecting the filtering that may be in place between the connector pin and the plane. See picture for a schematic example.

Place a ferrite in series with the cable shield pins near the USB connector socket to keep EMI from getting onto the cable shield. The ferrite bead between the cable shield and ground may be valued between 10 W and 50 W at 100 MHz; it should be resistive to approximately 1 GHz. To keep EMI from getting onto the cable bus power wire (a very large antenna) a ferrite may be placed in series with cable bus power, VBUS, near the USB connector pin 1. The ferrite bead between connector pin 1 and bus power may be valued between 47 W and approximately 1000 W at 100 MHz. It should continue being resistive out to approximately 1 GHz, as shown in below.

No comments:

Post a Comment