While most of the high speed interfaces like USB are routed in multi layer boards in complex mother board kind of designs or any other commercial application boards, there might be cases where USB signal might have to be routed in 2-layer boards. Take the example of an USB to RS232 converter which is used world wide by the engineers, and is mostly designed in a 2-layer board to save cost. These designs work without any issues and it is important that following guidelines are followed for a USB2.0 interface.
- In the case of 2-layer boards, before routing any trace, first route the USB so that you have design margins maintained. When we say design margins, it is especially spacing of USB traces to other traces.
- Place the controller as close as possible to the connector.
- The trace spacing between D+ and D- must be such a way that required impedance is maintained. This meant you are controlling the impedance of the USB. The impedance between D+ and D- must be 90 ohms & D+ to GND, D- to GND must be 45 ohms.
- Routing the traces in parallel to achieve the required impedance is crucial, while there are some deviations. Designers have lot of questions when they fan out the USB signals from the connector or the controller. In this scenario, there is no way required parallelism can be maintained in this scenario. Deviating from parallel routing for a very short distance is always acceptable. However, this need to be confirmed in either simulation or post prototype testing.
- If the PCB designer has concerns on impedance controlled routing, he can suggest the designer to have a series resistors on the USB lines so that they can be used layer for impedance matching and suppressing any reflections. Designer might already have used series resistor on D+ and D- lines.
- Length matching of D+ and D- must still be achieved. The skew should not exceed 50 mils for a USB2.0 interface
- Even though it is two layer board, for USB signals, prefer to have continuous ground on the opposite layer of USB routing so that there is continuous reference plane.
- ESD diodes are to be placed as close as possible to the connector. Placement of ESD diodes adds a stub on the D+ and D- lines. Do not have a stub more than 200 mils on these lines.
Skew allowed for a USB2.0 interface:
Maximum Data Rate of USB2.0 = 480Mbps
Minimum rise and fall time of high-speed USB2.0 signal = 500ps (As per USB 2.0 Specification )
The skew must be less than 1/10th of the maximum rise time which meant maintain within 50ps.
Let us assume we want to maintain 5% skew within the D+ and D-. As the USB2.0 Maximum data rate is 480Mbps, 5% of the rate is 0.05*(1/480M) = 0.1ns = 100ps
Equivalent Dielectric constant for micro strip is --- (0.64 Er+ 0.36) = (0.64 * 4 + 0.36) = 2.92
For routing on the top layer for a FR4 laminate is, +/- (100/(85*SQT(2.92)) = +/-0.688 in = +/- 688 mils.
]]>
0 Comments