USB-C: Cables, Connectors, and Circuit boards
Power delivery in USB-C coexists with SuperSpeed digital data. To reach the potential of this interface, first understand how the cables and connectors influence the PC Board layout requirements.
USB-C Cables - Are you confused yet?
There is not a single standardized USB-C cable. Each cable is tailored for its application, and electronically identified. High current applications require thicker gauge copper. Cable length is also limited by the application, due to both power loss and signal attenuation at high data rates.
The USB-C cable has 8 coax or 4 twinax high speed data connections. The lines are differential, providing 4 lanes of digital signals, with 2 in each direction. Each lane can carry 5Gbps or more data. These high data rates require length-matching and impedance control. A legacy USB 2.0 interface is also included. There are also two wires for a sideband, which can be another type of communication. For example, analog headphone connections are possible. The power wire Vbus can carry up to 3 Amps of current and 20 Volts. Configuration happens on the Config Channel. In earlier versions of the specification, there were two configuration wires. New versions remove one of these and provide Vconn instead, which can provide more power. There are two dedicated ground wires, and ground current also flows in the coaxial shields.
The USB specification is freely available from usb.org. It describes many possible cables, including specialized cables for USB 2.0, HDMI, high-speed data, and power-only.
|The micro-coax cables could easily be mistaken for ordinary wires. They have an insulating jacket, and inside is a braided shield that hides another insulated wire. This inner wire carries the data. Two matched micro-coax cables create a single high-speed differential data line. One coax carries the signal, and the other carries a negative copy of the same signal.
|Another implementation of the pair of data lines is twinaxial (twinax), where both the positive and the negative copies of the signal share the same shield. It is easier to match lengths in this type of wire, and it will probably be the more popular of the two alternatives.
The cables also include ground connections, buried components such as bypass capacitors, and cable ID circuits. This helps avoid device damage and reduces EMI emissions.
The connector design takes into account the EMI requirements for high-power and high-speed design. It has a grounded shell. The shell tabs solder to the board, and require slots. These slots add complexity to PC board fabrication.
Connector types include surface mount, mixed surface-mount and through-hole, through-hole, rugged, and mid-mounted.
The mid-connector saves height by sitting inside a board cutout. Be sure to consider board panelization before using this type of connector.
The connector pins ride inside grooves on a wafer made of plastic. The pins have different lengths so that power can be applied before the signals are connected.
Connector housings are available in ruggedized forms. A mixed through-hole and surface-mount connector provides additional ruggedness while also improving the layout of two-layer designs. Even more rugged connectors are cast from aluminum, and can be watertight.
The strength of the cable is limited. The intent is for the cable to break before the connector. Stress on the cable connection is typically from bending. For small amounts of bending, the cable is undamaged.
Up to a torque of 0.75 Newton-meters (N-m), the cable is designed to bend without damage to the cable or the connector. At some torque between 0.75 N-m and 2 N-m, the USB plug will break. The breaking point is defined as the point when the cable weakens. The curve in the graph shows the tragedy of a broken $30 cable. This happens before the connector in the device breaks, and the fragility of the cable should save the more expensive device from breaking. To ensure this is the case, the mechanical strength of the board can be simulated using finite element analysis.
DFM for High-Speed Digital PCBs
USB-C Printed Circuit Board Layout
The Paddle is a prototyping board and reference design. It brings out the SuperSpeed data lines, the USB 2.0 interface, and provides Power Delivery.
The symmetry of the top and bottom sides is not a coincidence. USB Type-C is a reversible plug, with no preferred bottom or top. Power, grounds, and signals appear on both sides, so that reversing the connector can be unwound by the circuitry on the board.
Most of the pins are duplicated so that the connector works in both orientations. For the SuperSpeed digital connections, the signal lanes are swapped. For applications where software can't untangle the bits, IC switching circuits can swap the signals again.
An older version of the specification had two configuration pins, Config1 and Config2. In the latest USB-C specification, there is a single configuration pin, and Vconn serves a variety of other functions, including providing more power.
USB-C Power Delivery
When a device first powers up, it gets a 5V supply with 500mA of current. This is an increase in default power over previous USB generations. For devices that need more current or voltage, a combination of Power Delivery hardware and a software negotiation process convinces the host system to increase the voltage and current. The available power is granted as increments of current at a fixed voltage. When the current reaches the limit of 3 Amps, a higher voltage is activated and the maximum current is reduced to provide the same amount of power.
Routing SuperSpeed + Traces
The SuperSpeed 5GHz differential signal pairs require matched length routing and impedance control. The maximum skew between the positive and negative signals in the cable is 100ps, and the printed circuit board should not add much to this. The FUSB340 is a 10Gbps SuperSpeed switch, and it has a typical skew of 6ps. Keeping the routing skew down to about 6ps requires lengths matched to about 1mm.
The differential impedance must be kept between 75 Ohms and 105 Ohms. Traces should be kept as short as possible, because inexpensive printed circuit board materials are lossy at high frequencies.
It is best to keep the traces on a single layer. If multiple layers are used, the length on each layer needs to be matched. This accounts for the differences in signal propagation velocity between layers. Vias routed to inner layers, especially on thick boards, create transmission line stubs that will harm signal integrity. Vias can be back-drilled to remove the stub.
Through-hole connector pins should not stick through the bottom of the board, since this also creates a transmission line stub. The connector pins need to be about the same length as the thickness of the board. If the leads are too long, they will require manual lead trimming, and this is a production nightmare. Leads that are not long enough to reach the bottom side of the circuit board will have soldering problems.
Calculation of the trace width and spacing needed for high-speed differential lines goes beyond simple rules of thumb or design curves. Signal integrity analysis tools include a 2D field solver that can help design the traces and spaces. Analysis is limited by the reality of board fabrication, which doesn't always conform to ideal geometries and dielectrics. It is a good idea to work with your PCB vendor to find a stackup that meets your needs. Differential test coupons added to PCB panels enable the bare-board manufacturer to verify that boards will meet the requirements.