Silicon Laboratories EFM32 Instruction Manual

AN0046: USB Hardware Design Guidelines
This application note gives recommendations on hardware design for implementing USB
host and device applications using USB capable EFM32 microcontrollers along with
some example schematics for different applications.
KEY POINTS
• Example Schematics for a variety of
applications
• PCB Design Guidelines for new
applications
silabs.com | Building a more connected world. Rev. 1.02

1. Introduction
Some EFM32 microcontrollers, for instance selected members of the Giant Gecko and Leopard Gecko families, offer on-chip USB sup-
port. The USB peripheral embedded on these devices include the USB PHY and an internal voltage regulator, thus requiring only a
minimum number of external components. The on-chip voltage regulator's primary purpose is to power the EFM32 USB PHY. But as it
can deliver more current than the EFM32 needs, it can be used to power other components as well, even in non-USB applications. This
can be very useful when component cost or PCB area is of concern.
This document will explain how to connect the USB pins of an EFM32 microcontroller, and will give general guidelines on PCB design
for USB applications. First some quick rules-of-thumb for routing and layout are presented before a more detailed explanation follows.
The information in this document is meant to supplement the information already presented in Energy Micro application notes AN0002
Hardware Design Considerations and AN0016 Oscillator Design Considerations, and it is recommended to follow these guidelines as
well.
The EFM32GG-STK3700 has been tested and passes the requirements as a USB Device. A test report confirming this is attached.
AN0046: USB Hardware Design Guidelines
Introduction
silabs.com | Building a more connected world. Rev. 1.02 | 2

2. USB Connection
This section gives a brief overview of the different USB roles an EFM32 Microcontroller is capable of. For more in-depth details, please
refer to the device family reference manual.
USB can be operated in 2 different modes; host or device, with hub being a special version of a USB device. A supplement to the USB
standard introduces "On-The-Go" mode, which enables a USB product to operate as either a host or a device depending on which kind
of controller is in the other end of the cable. A typical example for this would be a smartphone or a tablet that can both connect to a
computer as a USB Mass Storage Device, or act as a host if a memory card reader or a USB memory stick is connected.
A USB capable EFM32 microcontroller can operate as a host, a device or as an OTG dual role device. EFM32 microcontrollers do not
support operation as a USB hub. The EFM32 USB stack supports host mode and device mode, but not OTG mode.
2.1 EFM32 USB Pin Descriptions
The USB peripheral on EFM32 microcontrollers feature the following pins:
USB_DP - Data line
USB_DM - Inverted data line
USB_VBUS - Sensing if VBUS is connected.
USB_VBUSEN - VBUS Enable, a control signal for enabling VBUS in host applications. Connect to external VBUS switch.
USB_DMPU - Data Minus Pull-Up, a control signal for enabling external 4.7 kohm pull-up on USB_DM for low-speed operation. If VDD
is 3.3 V pull-up may be connected directly to USB_DMPU pin.
USB_ID - ID for determining which device should act as bus master in a link between two OTG Dual Role devices. Connect to ID pin on
USB Micro-AB receptacle.
USB_VREGI - Voltage regulator input.
USB_VREGO - Voltage regulator output.
AN0046: USB Hardware Design Guidelines
USB Connection
silabs.com | Building a more connected world. Rev. 1.02 | 3

2.2 EFM32 as USB Host
In host mode, the EFM32 acts as the bus master and is responsible of enumerating the USB devices, a process that includes inquiring
connecting devices for configuration information and assigning them an address on the USB bus. The USB host also controls data flow
on the bus by sequentially polling all devices for data, meaning that no device can transmit on the bus without a host request.
A USB host must be able to supply power to a connected USB device through the +5 V VBUS line.
EFM32
USB_DP 15 R VBUS
D-
GND
D+
USB_DM
USB_DMPU
USB_ID
USB_VBUS
USB_VBUSEN
USB_VREGO
USB_VREGI
VSS
VDD
USB Series A
receptacle
3.0 – 3.6 V 5.0 V
15 R
Connector
shield
SW
OC
EN
Vin
Vout
GPIO
1 µF
> 96 µF
Figure 2.1. USB Host Schematics
When designing hardware for USB Host, remember the following:
• Use a 48 MHz (2500 ppm) crystal.
• Use a ferrite bead for VBUS. Place near receptacle.
• Use a switch that can shut off VBUS if current exceeds 500 mA.
• Provide at least 96 uF decoupling capacitance on VBUS. Place near USB receptacle.
• Terminate D+ and D- with 15 ohm serial resistors. Place near EFM32.
• Use an ESD protection device. Place near USB receptacle.
• Select a USB Series A type receptacle.
2.3 EFM32 as USB Device
USB devices are bus slaves that provide functionality to the USB host. Devices must provide configuration information to the host so
that the host can configure the connection. Devices are separated in different classes depending on their functionality. Two different
types of device classes exist; hubs and functions. Hubs provide a host with more attachment points, while functions provides additional
functionality. Examples of functions are human interface devices, mass storage devices and communication devices.
USB devices will transmit data or control information over the bus when requested by the host. EFM32 microcontrollers can not operate
as a USB hub device. As a USB host provides +5 V over the VBUS line, a USB device can either be powered over the USB cable, or it
can be self powered. The following sections present schematics for how to connect an EFM32 as both a bus powered device and a self
powered device. Please refer to the USB specifications for details on how much current can be drawn over the USB bus for different
configurations.
AN0046: USB Hardware Design Guidelines
USB Connection
silabs.com | Building a more connected world. Rev. 1.02 | 4

2.3.1 Self Powered Device
EFM32
USB_DP 15 R VBUS
D-
GND
D+
Connector
shield
USB_DM
USB_DMPU
USB_ID
USB_VBUS
USB_VBUSEN
USB_VREGO
USB_VREGI
VSS
VDD
USB Series B,
USB Series Mini-B or
USB Series Micro-B
receptacle
1.85 – 3.6 V
15 R
1 µF
4.7 µF
Figure 2.2. USB Self Powered Device Schematics
When designing hardware for a self powered USB Device, consider the following:
• Use a 48 MHz (2500 ppm) crystal.
• Use a ferrite bead for VBUS. Place near receptacle.
• Provide at least 4.7 uF decoupling capacitance on USB_VREGI. Place near EFM32.
• Keep total load capacitance on VBUS below 10 uF
• Provide at least 1 uF decoupling capacitance on USB_VREGO. Place near EFM32.
• Terminate D+ and D- with 15 ohm serial resistors. Place near EFM32.
• Use an ESD protection device. Place near USB receptacle.
AN0046: USB Hardware Design Guidelines
USB Connection
silabs.com | Building a more connected world. Rev. 1.02 | 5

2.3.2 Bus Powered Device
EFM32
USB_DP 15 R VBUS
D-
GND
D+
Connector
shield
USB_DM
USB_DMPU
USB_ID
USB_VBUS
USB_VBUSEN
USB_VREGO
USB_VREGI
VSS
VDD
USB Series B,
USB Series Mini-B or
USB Series Micro-B
receptacle
15 R
1 µF
4.7 µF
Figure 2.3. USB Bus Powered Device Schematics
When designing hardware for a bus powered USB Device, consider the following:
• Use a 48 MHz (2500 ppm) crystal.
• Use a ferrite bead for VBUS. Place near receptacle.
• Provide at least 4.7 uF decoupling capacitance on USB_VREGI. Place near EFM32.
• Keep total load capacitance on VBUS below 10 uF
• Provide at least 1 uF decoupling capacitance on USB_VREGO. Place near EFM32.
• Connect USB_VREGO to VDD.
• Provide decoupling capacitance on VDD as per AN0002 Hardware Design Considerations.
• Terminate D+ and D- with 15 ohm serial resistors. Place near EFM32.
• Use an ESD protection device. Place near USB receptacle.
AN0046: USB Hardware Design Guidelines
USB Connection
silabs.com | Building a more connected world. Rev. 1.02 | 6

2.3.3 Low-speed
Speed identification of USB devices is done with a pull-up on one of the data lines. A low-speed capable device is identified by a 1.5
kohm pull-up resistor on the D- line. The internal pull-up resistor on EFM32 microcontrollers is approximately 2.2 kohm, so an external
4.7 kohm resistor must be placed in parallel to be standard compliant. This resistor should be connected to the USB_DMPU pin so it
can be switched on and off by the USB PHY.
Even if omitting the external pull-up resistor will most likely work, it will not be USB compliant because the internal resistor value is
outside the USB specification.
It should also be noted that according to USB specification, low-speed mode is defined to support a limited number of low-bandwidth
devices, such as mice. Low-speed devices are not allowed to use standard USB cables, and a separate specification for low-speed
cables exist.
EFM32
USB_DP 15 R VBUS
D-
GND
D+
Cable
shield
USB_DM
USB_DMPU
USB_ID
USB_VBUS
USB_VBUSEN
USB_VREGO
USB_VREGI
VSS
VDD
USB Captive Cable
15 R
1 µF
4.7 µF
4k7
Figure 2.4. USB Low-speed Device Schematics
When designing hardware for a Low-speed USB Device, consider the following:
• Use a 48 MHz 2500 ppm crystal.
• Use a ferrite bead for VBUS. Place near receptacle.
• Connect a 4.7 kohm resistor between USB_DMPU and D-
• Provide at least 4.7 uF decoupling capacitance on USB_VREGI. Place near EFM32.
• Keep total load capacitance on VBUS below 10 uF
• Provide at least 1 uF decoupling capacitance on USB_VREGO. Place near EFM32.
• Terminate D+ and D- with 15 ohm serial resistors. Place near EFM32.
• Use an ESD protection device. Place near USB receptacle or where the cable connects to the PCB.
• Do not use a standard USB receptacle.
In the above schematics, a bus powered device is shown. A low speed device may also be self powered, but if VDD is below
USB_VREGO (3.3 V) the external pull-up should be connected to USB_VREGO instead of USB_DMPU and a switch should be used to
turn it on or off through USB_DMPU. If this is not done, there will be a leakage current from VREGO to VDD through the pull-up.
AN0046: USB Hardware Design Guidelines
USB Connection
silabs.com | Building a more connected world. Rev. 1.02 | 7

2.4 EFM32 as USB On-The-Go Dual Role Device
On-The-Go Dual Role Device (OTG) is not yet supported in the EFM32 USB stack, but EFM32 hardware is OTG capable.
When operating as a OTG Dual Role Device, a USB product is capable of operating both as a USB host and a USB device. A dual role
capable device must use a Micro-AB receptacle which can accept both a Micro-A plug and a Micro-B plug. Two dual role devices can
be connected together with a cable that has a Micro-A plug in one end and a Micro-B plug in the other end. In this case the device
where the Micro-A plug is inserted will act as host and must provide +5 V on VBUS. The plug type is detected by the ID pin, which is
shorted to GND on a Micro-A plug.
EFM32
USB_DP 15 R VBUS
D-
GND
D+
USB_DM
USB_DMPU
USB_ID
USB_VBUS
USB_VBUSEN
USB_VREGO
USB_VREGI
VSS
VDD
USB Series Micro-AB
receptacle
< 6.5 µF
3.0 – 3.6 V 5.0 V
15 R ID
SW
GPIO OC
EN
Vin
Vout
Connector
shield
1 µF
Figure 2.5. USB On-the-Go Dual Role Device Schematics
When designing hardware for an OTG Dual Role Device, consider the following:
• Use a 48 MHz 2500 ppm crystal.
• Use a ferrite bead for VBUS. Place near receptacle.
• Connect the ID pin on the receptacle to USB_ID
• Ensure that total capacitance on VBUS is less than 6.5 uF
• Provide at least 1 uF decoupling capacitance on USB_VREGO. Place near EFM32.
• Terminate D+ and D- with 15 ohm serial resistors. Place near EFM32.
• Use an ESD protection device. Place near USB receptacle or where the cable connects to the PCB.
• Use a USB Series Micro-AB receptacle.
AN0046: USB Hardware Design Guidelines
USB Connection
silabs.com | Building a more connected world. Rev. 1.02 | 8

3. PCB Design Guidelines
This section presents some basic guidelines for high-speed PCB design as well as some specific rules of thumb for USB full-speed
design.
3.1 Recommended Routing Rules of Thumb
• Route D+ and D- as 90 ohm differential pair
• Always provide a good return path (ground) for current
• Do not route over a gap in the reference plane
• Keep away from the edge of the reference plane
• Keep skew less than 400 ps
• Route D+ and D- on top layer
• Route D+ and D- as short as reasonably possible
3.2 PCB Stackup
When designing high speed signal traces on a PCB, thought must be given to the PCB stackup. The two common approaches are to
either route high speed signals on an inner layer, or to keep them on the top layer. The advantage of using an inner layer is improved
noise immunity and to avoid any track impedance discontinuities when routing the signal under components, connectors etc. The bene-
fits with outer layer routing is to avoid vias which easily cause discontinuities in the return current path unless special care is taken. For
USB signals on EFM32 microcontrollers the preferred solution is normally to route the signal on an outer layer, as PCB traces usually
are short.
Independently of whether the signals are routed on an inner or outer layer, they should always be routed over a solid reference plane.
Thus the PCB should have minimum 2 layers.
3.3 Routing
When a signal trace on a PCB is long relative to the highest frequency component of the signal, transmission line effects must be taken
into consideration. The transition between when a wire should be modeled as a transmission line and a wire with "no length" is gradual,
but common practice is to apply transmission line models when the trace length is more than 1/10th of the wavelength of the highest
frequency component on the trace. For traces shorter than this, it is safe to assume that the voltage level is the same over the entire
trace.
For digital signals the shortest wavelength is dependent on the signal bandwidth which again depends on the shortest rise and fall
times. Faster rise times equals higher frequency content. A common approximation is that
BW ≈0.35
tr
where tr is the minimum rise time from 10-90%. USB specifies a minimum rise time of 4 ns, which equals a maximum signal bandwidth
of 87.5 MHz or a minimum wavelength of 1.7 meters on a typical PCB trace. Thus if PCB traces are shorter than 170 mm, it can be
argued that the characteristic impedance of a track is not important. However, good design practice is to route USB signals as an impe-
dance matched differential pair according to specification.
AN0046: USB Hardware Design Guidelines
PCB Design Guidelines
silabs.com | Building a more connected world. Rev. 1.02 | 9

3.3.1 Differential Pairs
The USB data lines, D- and D+, should be routed as a differential pair. The trace impedance should be matched to the USB cable
differential impedance, which is nominally 90 ohms for the signal pair.
The impedance of a signal track is mainly determined by its geometry (i.e. trace width and height above the reference plane) and the
dielectric constant of the material between the traces and a reference plane. When two tracks are closely spaced, they will be coupled
and the differential impedance will also be dependent on the distance between the two tracks comprising the pair.
In general one can say that if the two traces of a differential pair is spaced far apart, the differential impedance will be twice the impe-
dance of each trace. I.e. the two traces can be considered a shunt impedance. When the distance between the two traces is reduced,
coupling between the traces will cause the differential impedance to decrease. Thus to create a differential pair with 90 ohms impe-
dance, the single ended impedance of each trace should be above 45 ohms. Reducing the trace width will increase the single-ended
impedance while reducing the distance between the traces in a pair reduces the impedance. This allows routing of very closely spaced
differential pairs that use little PCB area. Note, however that thin traces will be more difficult to manufacture, and that for high frequen-
cies loss due to skin effect comes into play.
Most PCB design tools support differential pairs, and can create such pairs with specified parameters. If such a tool is not available,
there are many online impedance calculators that can calculate track parameters.
To avoid differential imbalance, skew (or trace length difference) between the two traces in a differential pair should be under control. A
common rule of thumb is to keep the skew less than 1/10th of the fastest rise time. For USB full-speed this translates to 400 ps or 60
mm. However, this is the total skew over the entire communication link so skew in the USB cable as well as in the other communicating
party must also be included. According to the USB specification the maximum allowed skew in a cable is 100 ps, which leaves a maxi-
mum of 300 ps (45 mm) of skew to be distributed amongst the host and device. Still, as you never know the characteristics of the other
end, good design practice is to keep skew at a reasonable minimum.
When high speed signals are routed from one layer to another, care should also be taken to provide a path for the return signals. Re-
member that even differential signals use a reference plane as return path. This is particularly important when designing PCBs with
many layers.
TOP
GND
BOTTOM
GND
Signal
path
Return
current
path
Figure 3.1. Changing layers on PCB
Stubs should also be avoided as they may cause signal reflections. For USB, this is seldom a problem as the data traces are point-to-
point. If a test point is desired, the signal should be routed through the test point, in a fly-by manner, rather than having a long trace
from the trace to the test point.
Figure 3.2. Recommended routing of test points
AN0046: USB Hardware Design Guidelines
PCB Design Guidelines
silabs.com | Building a more connected world. Rev. 1.02 | 10