AMWx06 Hardware Design Guide

• Overview
• Schematic Design
  • Power / Bypass Capacitors
  • UART Connection
  • Debug Header
  • Antenna Connection
• PCB Layout
  • PCB Layer Stack-up
  • Antenna/RF Routing
  • Ground
  • Power

Overview

The Zentri AMWx06 Wi-Fi module (AMW006, AMW106) is easily integrated into products to enable wireless and cloud connectivity. The module is designed to use very few external components, while still allowing the flexibility needed to cover most product use cases. While easy to use, there are a few guidelines and recommendations that must be followed in order to achieve optimal range and RF performance. Even after following the guidelines outlined in this document, Zentri recommends submitting the final design for review before prior to fabrication. A design review by Zentri’s experienced hardware design team is guaranteed to save you time and unnecessary debugging difficulties during board bringup, board testing and certification prior to production.

Schematic Design

Figure 1. AMWx06 Schematic Symbol

Power / Bypass Capacitors

The AMWx06 is designed primarily to run from a 3.3V power supply. The module draws transient currents up to 400mA. As such, the main power regulator should be designed to handle approximately 500mA for the Wi-Fi section of the board. A 500mA regulator provides enough headroom to cater for system inefficiencies and during extremes of temperature and voltage. Failure to provide an adequately sized power supply can create abnormal behavior that may be difficult diagnose including brownouts, partial resets, dropped characters, poor radio performance, and more.

VDD_MCU (Pin 10) is used to power the microcontroller section of the module. Zentri recommends 100nF and 10μF capacitors are used on this supply to help filter any switching transients created by the MCU. Both capacitors should be placed as close as possible to the pin. VBAT is connected to the battery backup section of the module. This supply is used during low power operation of the module. Zentri recommends a 100nF capacitor is used on this supply to help filter any switching transients created by the MCU. The capacitor should be placed as close as possible to the pin.

VDD_WIFI is used to power the Wi-Fi section of the module. Zentri recommends a 100nF and 10μF capacitor are used on this supply to help filter any switching transients created by the module. The capacitors should be placed as close as possible to the pin.

All capacitors should be of type X5R or better.

The VDD_MCU, VBAT, VDD_WIFI supplies are not connected on the module. For normal use cases, all three power supplies should be connected to 3.3V.

Table 1. Power Supply Specifications

UART Connection

The primary communications interface with the AMWx06 is a 4-wire serial UART connection. Zentri highly recommends that all 4 wires are connected to enable hardware flow control. Hardware flow control minimizes the likelihood of dropped data on the interface.

A secondary 4-wire UART may also be used for debug if required. Only 2 wires are typically needed on this interface since debug information is not critical. The UARTs nominally operate at 115200 baud, with 8 data bits, no parity and 1 stop bit.

All of the labels on the Zentri AMWx06 schematic are written from the perspective of the module. For instance, UART_TX is the transmit output of the module, UART_RX is the receive input of the module. The following table details UART connections.

Table 2. UART Connections

Debug Header

Zentri highly recommends a footprint for a Zentri debug/programming header is added to the design. A debug header can dramatically speed up debug / reprogramming issues that may arise during product development.

The recommended debug header is a small, 10 pin through hole, 50mil pitch header from Samtec, part number FTSH-105-01-F-D-K. Surface mount and hybrid variants are also available to suit most mechanical restrictions. Zentri hardware exclusively uses the debug header shown in Figure 2:

Figure 2. Debug Header Symbol

The UART connection may be connected to either UART interface. If the signals are shared with a host microcontroller, ensure a series resistor is added between the module and host MCU, and that the debug header connects directly to the module. This will ensure that the debug header can always gain control of the signals. See the example schematic in Figure 3.

Figure 3. Debug Header Reference Schematic

Antenna connection

The AMWx06 module is designed to work with (and is certified for) a variety of different antennas including Whip, PCB trace and ceramic chip antennas. Each antenna type has specific benefits and drawbacks, so the choice of antenna is dependent on the product requirements.

Tuning the antenna directly is the most optimal method of optimizing RF performance. This is normally done by trimming the length and size of the antenna features. If it is not possible to tune the antenna due to certification or physical restrictions, a lumped element “PI” network should be added to the antenna path. This will enable the impedance ‘seen’ by the module to be optimized to match the required 50 Ohms. Each method of antenna tuning has its limitations, so it is recommended that a “PI” network is added during prototype stages of the design.

If one of the antenna connections is not used, it is recommended to terminate the connection with a 49.9 Ohm resistor. Termination with of the unused port is not mandatory, but doing so will minimize spurious noise coupling into the receiver.

The following diagrams show some of the possible combinations.

Figure 4. u.FL Connector and a Ceramic Chip Antenna

Design file corresponding to Figure 4 (Gerber format)

Figure 5. PCB Trace Antenna and Termination Resistor

PCB Layout

Designing a PCB that uses an AMWx06 module is no different to designing a module with any high frequency RF circuit, radio design guidelines should be adhered to in order to achieve the best result. The main areas to pay particular attention to include: antenna connections, power supply routing and ground connections/stitching.

PCB Layer Stack-up

Zentri recommends a 4-layer, 50 Ohm impedance controlled stack-up is used for any designs using the AMWx06. The PCB stack-up should look as follows:

Module/Signal
-------------
  Ground
-------------
Power/Signal
-------------
   Signal

Contact your PCB supplier to find out which layer and trace thickness is needed in order to obtain the 50 Ohm impedance (at 2.4GHz) as this varies from vendor to vendor. For a standard 62mil thick PCB, try to use a 10mil trace for the 50 Ohm connections.

It is still possible to use a 2-layer stack-up, however this should only be done on very simple designs that do not use many IO connections and only use u.FL connectors with very short RF traces. It is typically not possible to maintain a 50 Ohm impedance on a two layer board while keeping RF traces to a reasonable width.

Antenna/RF Routing

PCB layout is all about compromise and priorities. Following these guidelines will help create an optimal result, however mechanical/budgetary/size constrains often prevent an ideal layout. The final design ultimately comes down to some experimentation to determine if the results and performance are adequate for the product.

The following list outlines areas of particular importance:

• RF traces should be kept as short and straight as possible.
• Traces should not have sharp bends or sharp transitions through components e.g. through a capacitor placed perpendicular to the trace.
• Avoid routing under traces on other layers. If traces must cross, ensure the trace crosses at 90 degrees to minimize capacitive coupling between traces.
• RF traces should be routed on a layer above a solid ground plane (special rules apply for PCB trace antennas, do not place copper underneath PCB antennas).
• Keep RF traces away from noisy signals and power supplies.
• Make sure antenna clearance rules are strictly followed. If these rules are violated, the tuning and efficiency of the antenna will be adversely impacted which will impact radio range.
• For ‘PI’ matching components (L / C / R), use components that are sized close to the nominal trace width. e.g., for 10mil RF traces, use 0402 components, for 5mil trace width (on very thin PCB’s) use 0201 components. Try to avoid larger 0603 or 0805 parts as they have larger parasitic capacitance and create impedance mismatches.

There are numerous different combinations of antennas that can be used with the AMWx06, however here is a selections covering a few of the use cases. These diagrams can be used as guides on how to place the antennas, add grounding, route RF traces etc. Note that only the top layer and power routing (buried layer, in blue) are shown.

Figure 6. PCB Trace antenna + termination resistor

Download design file corresponding to Figure 6 (Gerber format)

Figure 7. Two U.FL connectors. One with a "PI" matching network

Download design file corresponding to Figure 7 (Gerber format)

Figure 8. Two Orthogonal PCB Trace Antennas

Download design file corresponding to Figure 8 (Gerber format)

Ground

Good grounding is critical for obtaining optimal RF performance. The following guides will help achieve the best results:

• Place a solid ground fill under the module and RF section (NOT directly under the antenna!)
• Follow datasheet recommendations for polygon fill keep-out areas of antennas and connectors.
• Use ground fill on all layers near the AMWx06 and RF areas.
• Minimize routing under the module (especially high frequency and/or high current traces).
• Add lots of via stitching to shield the RF traces/component and also along the antenna/fill boundary as shown in the reference diagrams.
• Add a stitching via at the ground contact point for the PCB trace antennas.
• Add ground vias at every ground pad on the module.
• Use a direct connection to the ground pads of the RF matching components and connectors (no thermal relief).
• Do not cut the ground plane and definitely do not route the ground signal. Doing so may make the module "RF hot" and badly impact performance, even to the point of making the module fail to work entirely.

Power

Any noise on the power supply may be coupled into the RF section of the module and then radiated out of the antenna. This can impact receive sensitivity and cause the device to fail certification testing. Observing the following points will help to keep noise coupling to a minimum.

• Keep all common mode impedance to a minimum. This is done by star routing the high current supplies (VDD_MCU and VDD_WIFI) directly from the voltage regulator and bulk capacitance. Do not daisy chain the power supplies together with other devices using the same power supply (e.g. host microcontroller, display driver, etc.).
• All power traces should be a minimum thickness of 25mil (thicker is better). Thick traces minimize series resistance and power supply impedance.
• Use multiple vias to connect high current supplies (VDD_MCU and VDD_WIFI). This reduces via resistance and voltage drop.
• Ensure bypass capacitors are placed as close as possible to module power supply pins with smaller values closest.
• Route all power supply traces through capacitor pads and THEN to module pins, rather than to the module pin first as shown in Figure 6, Figure 7 and Figure 8.