Internal supply rails are generated by local switching or linear regulators from higher voltages. The example shown here starts from external 24 V, generates an intermediate 5 V rail and finally 3.3 V and 1.8 V rails for different subsystems using switching regulators.

This document does not focus on how to design a switching regulator, keep in mind general rules about current loops and check the data sheets. Also the document does not cover the basics for linear regulators.

When implementing a supply for an Ethernet PHY, stick to the guidelines given in the data sheet, in terms of capacitors and filtering on the supply rails. Typically you want to have two to three capacitors with different capacitance per supply pin as well as some bulk capacitance. On top of this, the recommendation is to have the option for some low pass filtering. Figure 2-2 shows a set of capacitors per pin and with R77 and R78 the option for filtering is given. Multiple capacitors with different capacitance and sizes are used to get a low impedance over a wide frequency range. There also different physical sizes from 0402 (for very high frequencies also 0201 or smaller) up to 0805 can help.

During (pre-)compliance tests you can see if there is a need to add additional filtering, for example, by using ferrite beads. If there is noise visible, correlating to frequencies used inside the device, or you can measure a lot of HF current going through this resistor (a near field probe can help), it can help to add a ferrite bead to keep this noise away from the power planes.

Figure 2-2 Power Supply Schematic

In terms of layout, there is an importance to have the components in the correct order and connected with wide and short traces. Every trace has parasitic elements, especially resistance, and inductance can be bad in this case. As a rule of thumb a trace of 1 cm has 10 nH of inductance. This does not sound much, but when looking at the impedance at 100 MHz, we have about 6 Ω, which is already significant. So a capacitor connected through a long and thin trace is useless for higher frequencies.

Also, the impedance of capacitors changes over frequency, as real capacitors have parasitics and do not behave like ideal capacitors. Typically, small capacitance are better designed for filtering high frequencies than high capacitance. Also, the physical size makes a difference, the smaller the better for high frequency, as the series inductance is lower. Also, stay away from through hole parts or electrolytic caps for filtering in this case.

Figure 2-3 shows the layout for this implementation, the trace from the pin is as short as possible and going to a bank of capacitors with increasing values. This bank is connected at the very end through a ferrite bead to the supply plane. Also think about the return path, every current going into a supply pins needs to go back somehow. This path also needs to provide a low impedance path to the same source. The typical approach of having a solid GND plane is a good design, when you also connect the return path of the IC and of the caps in a solid way. This means to have a set of vias as close as possible. Here you are limited by the manufacturing capabilities you want to pay for. Stay away from pads, so the vias and the pad are separated by the solder mask otherwise you can have problems when manufacturing the board. If you really want to have the vias in the pads, talk to your manufacturer upfront about this.

In some cases it can be necessary to have the capacitor on the other side of the PCB directly below the IC. This is also a good approach, but again, the via adds some inductance, a 0.2 mm vias in a 1.6 mm PCB has about 1 nH, so similar to 1 mm PCB trace.

Figure 2-3 Power Supply Layout