Maxim > Design Support > Technical Documents > Application Notes > Prototyping and PC-Board Layout > APP 4049
Keywords: MAX8660, PCB, printed circuit board, layout
APPLICATION NOTE 4049
MAX8660/MAX8661 PCB Layout Guide
May 29, 2007
Abstract: The MAX8660/MAX8661 evaluation kit provides an example that uses a one-sided printed
circuit board (PCB) layout to optimize performance. Whereas the evaluation kit PCB layout provides
optimal performance and eases evaluation, other layouts are also acceptable. This application note
provides a step -by -step procedure for achieving a reliable PCB layout with the MAX8660/MAX8661.
Introduction
The MAX8660/MAX8661 are highly integrated power-management ICs (PMICs). The high efficiency and
small size of these devices make them ideal for portable battery - powered applications, such as smart cell
phones, PDAs, and portable media players.
Good printed circuit board (PCB) layout is necessary to achieve optimal MAX8660/MAX8661
performance. The evaluation kit (EVKIT) for the MAX8660 provides an example layout that optimizes its
performance. For implementations that cannot utilize this layout, this application note provides
procedures and design tips for maximizing the performance of your MAX8660-based design.
MAX8660EVKIT
The MAX8660EVKIT has been provided as a PCB layout example and has the following characteristics:
Four layers
1oz copper
All components on one side of the PCB
5mil vias between layers 1 and 2 to route digital signals
The MAX8660/MAX8661 do not require a one-sided PCB layout—two-sided layouts are also acceptable.
The MAX8660EVKIT utilizes a one -sided PCB layout for the following reasons:
All dynamic switching currents for the step - down regulators are contained to the top layer of metal.
There are no dynamic switching currents that flow through vias.
Many designs use 8- to 12 -layer PCB designs. It is common to place noisy components such as
the PMIC on one side of the PCB, while placing sensitive components such as a GPS receiver on
the other side. Because the middle layers of the board are ground, they effectively isolate the two
sides from each other. The MAX8660EVKIT was created to be single-sided so that it can easily be
ported to these applications.
For lab evaluations, it is convenient to have all components on one side so they can all be easily
probed.
Additionally, having all components on one side allows the board to lie flat on the table, further
easing lab evaluation.
Page 1 of 7
To maintain a small PCB area, the evaluation kit utilizes blind microvias (5mil vias between layers 1 and
2) to route digital signals. Similar layouts can be achieved without these blind microvias at the expense
of area.
Maxim encourages MAX8660/MAX8661 users to follow the MAX8660EVKIT layout as closely as
possible. To facilitate this we provide the Gerber files¹ for the MAX8660EVKIT layout. For PCB designs
in which the MAX8660EVKIT layout cannot be adopted, this application note provides a step -by-step
procedure that can be followed to achieve a reliable layout.
Support Documents for this Application Note
MAX8660 data sheet
MAX8660EVKIT data sheet
MAX8660EVKIT Gerber files
Mechanical description of the board (Appendix)
PCB Layout Procedure for the MAX8660/MAX8661
The reference designators used in this section match the schematics shown in the EVKIT data sheet
(refer to Figure 4 in the MAX8660EVKIT data sheet). It is highly recommended that you consult the
layout within the EVKIT data sheet (Figures 5, 6, 7, 8, and 9 in the EVKIT data sheet) and these
recommendations at the same time.
The elements of this procedure are listed in order of importance. Items at the top are most important.
1. Step-Down Converter Input Bypass Capacitors
Place C12 between PV3(28) and PG3(26) as close as possible to the IC.
Place C11 between PV1(36) and PG1(34) as close as possible to the IC.
Place C15 between PV2(14) and PG2(16) as close as possible to the IC.
Place C18 between PV4(3) and PG4(5) as close as possible to the IC.
The step -down converter input bypass capacitors are the most critical components because
they carry discontinuous currents with a high rate of change (di/dt). Minimizing the inductance
between the step -down converter input bypass capacitors and the PVx and PGx pins is
critical. Install the input capacitors on the same side of the PCB as the
MAX8660/MAX8661 IC in order to minimize inductance. Placing the input capacitor on the
opposite side of the PCB as the MAX8660 IC is not ideal because the vias that are necessary
to connect the two halves of the PCB add inductance to this critical path.
The MAX8660/MAX8661 provide one buck converter on each side of the IC package, thereby
allowing buck input capacitors to be placed close to their PVx and PGx pins.
Each buck converter has a pinout with PVx, LXx, and PGx such that PVx and PGx are
separated by one pin. The pinout, along with the package’s pin pitch, makes a 0603 size input
capacitor ideal.
Connect each input capacitor ground terminal to the internal ground plane with multiple vias.
Multiple vias reduce resistance and inductance.
Connect each input capacitor positive terminal to the internal power plane with multiple vias.
Multiple vias reduce resistance and inductance.
2. IC Power Input, Ramp -Setting Resistor, and Low - Battery Comparator Components
Place C22 between IN(18) and AGND(19) as close as possible to the IC.
Place R10 next to C22.
Place R2 between LBF(21) and LBR(22) as close as possible to the IC.
Place R1 and R3 next to R2; keep the high -impedance nodes at LBF(21) and LBR(22) as
Page 2 of 7