返回首页
当前位置: 主页 > 互联网技术 > 网络管理 >

高速USB设计PCB布线要求

时间:2015-05-03 22:36来源:电脑教程学习网 www.etwiki.cn 编辑:admin

1-2 is omited, for more detail please refer to www.usb.org.

.......

3 Layout Guidelines

3.1 General Routing and Placement
Use the following general routing and placement guidelines when laying out a new design. These
guidelines will help to minimize signal quality and EMI problems. The high speed USB validation efforts
focused on a four-layer motherboard where the first layer is a signal layer, the second layer is power, the
third layer is ground and the fourth is a signal layer. This results in placing most of the routing on the
fourth layer closest to the ground layer, and allowing a higher component density on the first layer.
1. Place the high-speed USB host controller and major components on the unrouted board first.
2. With minimum trace lengths, route high-speed clock and high-speed USB differential pairs first.
Maintain maximum possible distance between high-speed clocks/periodic signals to high speed USB
differential pairs and any connector leaving the PCB (such as, I/O connectors, control and signal
headers, or power connectors).
3. Route high-speed USB signals on bottom whenever possible.
4. Route 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 by minimizing impedance discontinuities.
6. Do not route USB traces under crystals, oscillators, clock synthesizers, magnetic devices or ICs that
use and/or duplicate clocks.
7. Stubs on high speed USB signals should be avoided, as stubs will cause signal reflections and affect
signal quality. If a stub is unavoidable in the design, no stub should be greater than 200 mils.
8. Route all traces over continuous planes (VCC or GND), with no interruptions. Avoid crossing over
anti-etch if at all possible. Crossing over anti-etch (plane splits) increases inductance and radiation
levels by forcing a greater loop area. Likewise, avoid changing layers with high-speed traces as much
as practical. It is preferable to change layers to avoid crossing a plane split. Refer to Section 3.6 Plane
Splits, Voids and Cut-Outs (Anti-Etch) for more details on plane splits.
9. Separate signal traces into similar categories and route similar signal traces together (such as routing
differential pairs together).
10. Keep high-speed USB signals clear of the core logic set. High current transients are produced during
internal state transitions and can be very difficult to filter out.
11. Follow the 20*h thumb rule by keeping traces at least 20*(height above the plane) away from the edge
of the plane (VCC or GND, depending on the plane the trace is over). For the suggested stackup the
height above the plane is 4.5 mils. This calculates to a 90-mil spacing requirement from the edge of
the plane. This helps prevent the coupling of the signal onto adjacent wires and also helps prevent free
radiation of the signal from the edge of the PCB.
3.2 High Speed USB Trace Spacing
Use the following separation guidelines. Figure 3 provides an illustration of the recommended trace
spacing.
1. Maintain parallelism between USB differential signals with the trace spacing needed to achieve 90
ohms differential impedance. Deviations will normally occur due to package breakout and routing to
connector pins. Just ensure the amount and length of the deviations are kept to the minimum possible.
2. Use an impedance calculator to determine the trace width and spacing required for the specific board
stackup being used. For the board stackup parameters referred to in section 3.7 Layer Stacking, 7.5-
mil traces with 7.5-mil spacing results in approximately 90 ohms differential trace impedance.
3. Minimize the length of high-speed clock and periodic signal traces that run parallel to high speed USB
signal lines , to minimize crosstalk. Based on EMI testing experience, the minimum suggested spacing
to clock signals is 50 mils.
4. Based on simulation data, use 20-mil minimum spacing between high-speed USB signal pairs and
other signal traces for optimal signal quality. This helps to prevent crosstalk.

Image

             Figure 3 Recommended trace spacing (mils) for the stackup given in Section 3.7

3.3 High Speed USB Termination
Use the following termination guidelines.
1. High-speed USB designs require parallel termination at both the transmitter and receiver. For host
controller designs that use external termination resistors, place the termination resistors as close as
possible to the host controller signal pins. Recommend less than 200 mils if possible. Follow the
manufacturer’s recommendation for the termination value needed to obtain the required 45 ohm-toground
parallel HS termination.
2. For downstream ports, a 15 kW pull down resistor on the connector side of the termination is required
for device connection detection purposes. Note that this pull down might be integrated into the host
controller silicon. Follow the manufacturer’s recommendation for the specific part used.
3. A common mode (CM) choke should be used to terminate the high speed USB bus if they are need to
pass EMI testing. Place the CM choke as close as possible to the connector pins. See Section 5.1 for
details.
Note: Common mode chokes degrade signal quality, thus they should only be used if EMI is a
known problem.
3.4 High Speed USB Trace Length Matching
Use the following trace length matching guidelines.
High-speed USB signal pair traces should be trace-length matched. Max trace-length mismatch between
High-speed USB signal pairs (such as, DM1 and DP1) should be no greater than 150 mils.
3.5 High Speed USB Trace Length Guidelines
Use the following trace length guidelines.

                                                                  Table 1 Trace length guidelines

Image

 

3.6 Plane Splits, Voids and Cut-Outs (Anti-Etch)
The following guidelines apply to the use of plane splits, voids and cutouts.

VCC Plane Splits, Voids, and Cut-Outs (Anti-Etch)
Use the following guidelines for the VCC plane.
1. Traces should not cross anti-etch, for it greatly increases the return path for those signal traces. This
applies to High Speed USB signals, high-speed clocks and signal traces as well as slower signal
traces, which might be coupling to them. USB signaling is not purely differential in all speeds (i.e.
the FS Single Ended Zero is common mode)
2. Avoid routing of USB signals within 25 mils of any anti-etch to avoid coupling to the next split or
radiating from the edge of the PCB.
When breaking signals out from packages it is sometimes very difficult to avoid crossing plane splits or
changing signal layers, particularly in today’s motherboard environment that uses several different voltage planes. Changing signal layers is preferable to crossing plane splits if a choice has to be made between one
or the other.
If crossing a plane split is completely unavoidable, proper placement of stitching caps can minimize the
adverse effects on EMI and signal quality performance caused by crossing the split. Stitching capacitors are small-valued capacitors (1 mF or lower in value) that bridge voltage plane splits close to where high speed
signals or clocks cross the plane split. The capacitor ends should tie to each plane separated by the split.
They are also used to bridge, or bypass, power and ground planes close to where a high-speed signal
changes layers. As an example of bridging plane splits, a plane split that separates VCC5 and VCC3
planes should have a stitching cap placed near any high-speed signal crossing. One side of the cap should
tie to VCC5 and the other side should tie to VCC3. Stitching caps provide a high frequency current return
path across plane splits. They minimize the impedance discontinuity and current loop area that crossing a
plane split creates.
GND Plane Splits, Voids, and Cut-Outs (Anti-Etch)
Use the following guideline for the GND plane. Avoid anti-etch on the GND plane.
3.7 Layer Stacking
The following guidelines apply to PCB stack-up.
Four-layer Stack-Up
1. Signal 1 (top)
2. VCC
3. GND
4. Signal 2 (bottom, best layer for USB2)
The high speed USB validation motherboard used 7.5-mil traces with 7.5-mil spacing between differential
pairs to obtain 90W differential impedance. The specific board stackup used is as follows:
· 1 ounce copper
· prepreg @ 4.5 mils
· core @ 53 mils
· board thickness @ 63 mils
· _r @ 4.5
3.8 Component Placement

The following guidelines apply to component placement on the PCB.
1. Locate high current devices near the source of power and away from any connector leaving the PCB
(such as, I/O connectors, control and signal headers, or power connectors.) This reduces the length that
the return current travels and the amount of coupling to traces that are leaving the PCB.
2. Keep clock synthesizers, clock buffers, crystals and oscillators away from the high speed USB host
controller, high speed USB traces, I/O ports, PCB edges, front panel headers, power connector, plane
splits and mounting holes. This reduces the amount of radiation that can couple to the USB traces and
other areas of the PCB.
3. Position crystals and oscillators so that they lie flat against the PCB. Add a ground pad with the same
or larger footprint under crystals and oscillators having multiple vias connecting to the ground plane.
These will help reduce emissions.


4 Some Common Routing Mistakes
4.1 Stubs

A very common routing mistake is shown in Figure 4. Here the CAD designer could have avoided
creating unnecessary stubs by proper placement of the pull down resistors over the path of the data traces.
Once again, if a stub is unavoidable in the design, no stub should be greater than 200 mils.

Image

Figure 4 Creating unnecessary stubs

4.2 Poor Routing Techniques
Figure 5 demonstrates several violations of good routing practices for proper impedance control and signal
quality of high speed USB signaling.
Crossing a plane split
The mistake shown here is where the data lines cross a plane split. This causes unpredictable return path
currents and would likely cause a signal quality failure as well as creating EMI problems.
Creating a stub with a test point
Here is another example where a stub is created that could have been avoided. Stubs typically cause
degradation of signal quality and can also affect EMI.
Failure to maintain parallelism

Image

           Figure 5 Violation of proper routing techniques


Figure 5 is also a classic example of a case where parallelism was not maintained, when it could have been.
The red trace (the lighter trace farthest to the right with the “x” on it) shows the wrong way to route to the connector pins. The green trace (the darker trace in the middle) shows the correct way. Failing to maintainparallelism will cause impedance discontinuities that will directly affect signal quality. In this case it also contributes to the trace-length mismatch and will cause an increase in signal skew.

5 EMI/ESD Considerations
The following guidelines apply to the selection and placement of common mode chokes and ESD
protection devices.
5.1 EMI - Common Mode Chokes
Testing has shown that common mode chokes can provide required noise attenuation. A design may
include a common mode choke footprint to provide a stuffing option in the event the choke is needed to
pass EMI testing. Figure 6 shows the schematic of a typical common mode choke and ESD suppression
components (refer to Section 5.2 ESD
). The choke should be placed as close as possible to the USB connector signal pins.

Image

                                    Figure 6 Common mode choke

Examples of specific common mode chokes that were tested for signal quality and EMI with passing
results are given in Table 2. Other vendors make similar parts that may provide the same results but due to
limited time and resources they were not tested.

顶一下
(4)
100%
踩一下
(0)
0%
标签(Tag):高速USB设计 PCB布线要求
------分隔线----------------------------
------分隔线----------------------------
发表评论
请自觉遵守互联网相关的政策法规,严禁发布色情、暴力、反动的言论。
评价:
表情:
验证码:点击我更换图片
推荐内容