Wiznet makers

INTRO

I have completed documentation on the HW design for WIZnet's new chip, the W55RP20. 

We will focus on WIZnet's official module, the W55RP20-EVB-Pico.

POWER

First, let's look at the power section. The EMC performance can vary significantly depending on how this section is designed, so it must be done with care.

Pins related to the power of the W55RP20 include AVDD, IOVDD, VDD, VREG_IN, USB_VDD, DVDD, VREG_OUT, TOCAP, and 1V2O. Please refer to Raspberry Pi RP2040 Datasheet for VREG_IN, IOVDD, USB_VDD, and VREG_OUT Pin. 
 The VDD is the main power source of the W55RP20. It should be powered by 3.3V of noise-free power. A 1uF power stabilization capacitor must be fitted and a 0.1uF decoupling capacitor must be fitted on each pin.
 AVDD is involved in the Ethernet MDI line and ADC. Like VDD, a 1uF capacitor for power stability should be installed, and a decoupling capacitor of 0.1uF should be installed close to each pin.  In addition, it is recommended to isolate MDI from digital power sources. Therefore, AVDD recommends isolation from VDD. Likewise, AGND also recommends isolation from DGND. However, if a sufficient area of DGND is not supplied, it can adversely affect EMI-RE. It is important to design it to control EMI-RE and communication quality well. This part can be resolved by the bead design of DGND-AGND.
 1V2O is the power source of the internal Ethernet core, which is connected to the internal regulator and should never be connected to an external circuit. The correct design method is to install a decoupling capacitor of 0.1 uF.

Decoupling capacitors should be close to the chip. The image above is W55RP20-EVB-Pico. It is better to place it closer than the design in that image.

OSC

W55RP20 needs to design two OSCs. Since it is RP2040 + W5500, we need to design an OSC per chip. For 12MHz OSC of RP2040, see Raspberry Pi RP2040 Datasheet. It is best to use an oscillator that vibrates automatically when power is applied. However, if this is not the case, you should follow the above. When using X-TAL, the design line should have no vias. It should also be positioned as close as possible to the MCU. There should be no patterns or elements in the other layers that could affect the X-TAL.

The X-TAL used in the Raspberry Pi Pico board is an X-TAL with a unique specification. The load capacitance must be carefully checked and designed to ensure that the operation is not abnormal. For more information, please refer to Raspberry Pi RP2040 Datasheet. 

The CL of the W5500 X-TAL of the W55RP20-EVB-Pico is 18pF. The R25 is used for current limitation, but is set to 0 ohm on the W55RP20-EVB-Pico. R24 acts as a terminating resistor; in most cases, you do not need to change it.

Notice : The operating characteristics may vary depending on the characteristics of the selected X-TAL and the parasitic capacitance caused by the Artwork. 
Please design by considering load capacitance, parasitic capacitance, etc.

 X-TAL should be routed without via for as short a distance as possible. If there are other lines penetrating through, the behavior may be affected, so you should route them so that they are not affected as much as possible.

MDI Line

The circuit may change depending on the internal circuit configuration of the Ethernet socket. Make sure to refer to Datasheet and design the circuit in an appropriate way.

If you use an Ethernet socket that does not include a transformer, you must also design the transformer part of the circuit.

The TCT of the transformer, the GND connected to the RCT, and the GND connected to the longitudinal resistance of the TX and RX can be designed as AGND instead of the normal GND. This is for the separation of the MDI signal from the system GND noise, in which case the area of the AGND should be large enough. Otherwise, it is more advantageous to integrate AGND and system GND.

Option1 is a damping resistance against EMC. Resistance to prevent common mode noise and differential mode noise interference; if the resistance value is designed too large, the voltage level of the differential line may decrease, which may cause Ethernet communication problems.

The distance between RJ-45 and Chip should be as close as possible.

Because the Tx, Rx signals are differential signals, each line must be of the same length. If the lines are formed differently, the differential mode signal can switch to common mode noise, affecting EMI, and causing Ethernet communication to become a problem.

It is recommended that a GND pattern be placed between TX and RX so that there is no influence between the two lines.

If the distance between the two lines is wide enough not to affect each other, there is no need for GND Copper.

The Impedance of the Line depends on the GND processing. When designing this part, Impedance Matching is possible with line thickness and Clearance.

It is not good for other Digital Lines to pass through the TX and RX lines. It is not good to have a high frequency device around (OCS, etc.)

Minimum condition for Ethernet Impedance Line design.

The impedance of Ethernet is 100 ohms.

In order to design an accurate Impedance 100 ohm, you should ask the PCB manufacturer to design it.
(Impedance changes depending on Solder Mask, Oz, and process method.)