Required components, layout recommendations and best practices
The imp001 card makes developing Internet-connected hardware very simple. The imp001 contains the processor, WiFi and antenna. Your design needs to include a few inexpensive components, and make some simple layout and routing rules. If you follow these guidelines, you can expect excellent, reliable WiFi performance.
Your design will require the following in addition to the imp card:
It’s very important that your card socket does not have metal over the antenna area inside the imp card. Check the imp001 datasheet for more information on recommended parts.
Do not use an SD socket with metal over the antenna area, like this one
This (supported) SD socket does not cover the antenna area
The imp requires an Atmel ATSHA204A ID chip connected to pin 6 of the imp card. The ATSHA chip must be the 1-Wire variant; the I²C version is not supported.
This bypass capacitor helps stabilize the rail during major changes in load, such as when the imp turns on its WiFi transmitter. It also operates to filter noise out of the imp’s power supply rail. This is especially important as feedback of WiFi noise into the imp’s power supply rail will severely impact performance.
The imp001 socket and ATSHA204A ID chip on the Quinn reference design
Applying more load than this to the imp’s pins will damage the imp. If your design requires you to move more current around, use an imp pin to switch a FET or transistor.
Your design must not expose any of the imp pins to a voltage greater than VDD (the supply voltage provided to the imp). Consult the imp001 datasheet for more information on the imp001’s electrical characteristics and absolute maximum ratings.
The imp’s internal pull-up or pull-down resistors will be cleared when the imp reboots, and these nets will be tri-stated. This is also important for handling the behavior of your design when the imp is removed from the socket.
It’s very important that your design follow a few simple rules when it comes time to place and route your printed circuit board in order to take advantage of the imp’s simplicity and to maximize performance.
The imp001’s ground pins should have a clear path back to ground without running through many narrow traces or bottlenecking at a single via. While a via may be rated for much more DC current than your design calls for, the impedance of the ground path needs to be as low as possible to prevent noise from becoming a problem in your design. This applies to other parts of your design as well, so minimize ground impedance everywhere.
Use Ground Pours Flood ground on the top and bottom of your PCB to provide a good ground path to all components. The imp’s antenna tuning ‘expects’ a ground pour under the non-antenna portion of the card. If the ground pour is omitted, the antenna will be de-tuned. This will negatively impact range and performance, and may prevent your product from passing wireless certification.
Stitch ground planes around the edge of your board and throughout the interior of the board. Use more vias than you need for the DC current your circuit requires; this will lower the impedance of the ground paths and reduce noise.
Stitching vias used around the edges and throughout the interior of
the Kelly reference design to improve ground impedance
The antenna comes pre-tuned for best performance, but the tuning is applied with just air under the antenna. If you place anything under the antenna, you will de-tune the imp and reduce WiFi performance and range. Your ground pour should not go past the mechanical pads on either side of the SD socket.
Your bypass capacitor will dump noise to ground, but if the trace on the filtered side is long, it presents an opportunity for that trace to pick up noise again.
Bypass capacitor placed immediately
next to the VDD pins on the imp
This provides shielding for the antenna and helps get the best performance. Stitching vias should be spaced at 200mil or less. You should pour ground across the SD Card socket footprint between the mechanical pads near the open end of the slot, and keep all copper behind this line.
The top-layer ground pour stops at the mechanical pads on the Kelly reference design.
The imp protrudes past the edge of the board, keeping the FR4 from detuning the antenna.
A poorly-routed switching power supply will send noise all over the board and severely impact performance and range. This is easily avoided by following the recommended layout in the datasheet for nearly any switching power supply IC.
Recommended Layout for the TPS62172 Buck Regulator, as shown in TI’s datasheet
Noise on your board directly diminishes your WiFi performance and can prevent you from passing FCC certifications. Keep all noisy parts (switching power supplies, high-speed signalling) as far from the imp’s antenna as possible.
Routing signals in the correct order can significantly simplify a design:
Route high-speed signals directly and avoid vias By keeping the path between devices that communicate over a high-speed interface such as SPI direct and short, you minimize the possibility that noise will couple into the line, or that the signals on the line will couple into other parts of your design as noise.
Place your power supply and route VDD It’s generally a good idea to avoid vias on your power supply rail; these increase the impedance of the trace and create an opportunity for noise to impact your design.
Keep analog signals clear of noisy digital signals and route them as directly as you can Routing an analog signal right next to a digital signal creates an opportunity for digital noise to couple into the analog signal. Keep them apart and pour ground in between to provide some shielding.
Route GPIOs last A signal which is simply used to poll a button or toggle an LED does not need special considerations. If a GPIO signal crosses a higher-priority signal such as a SPI bus or an analog line, the lower-priority signal should via around the higher-priority one.