Embedded Systems
Products & Services

Home Services Products Resources About Contact

Javascript is used
on this Web site to
do things like open
pop-up windows
and to prevent
harvesters from
extracting PayPal
account info.

All material on
this Web site is
protected under
United States
and International
copyright law.

Liability for your
use of information
on this Web site is
strictly limited.

Trademarks used
on this Web site
are the property of
their respective

LTC is a registered
trademark of Linear

Five Switching Regulators in Three Square Inches

Switching Regulator PCB

Linear Technology makes some very highly integrated power management chips for cameras, PDAs, MP3 players, etc.  An example is the LTC3586, which includes five switching power regulators - one to charge the battery and the other four to provide a variety of supply voltages to the application circuit.  The customer wanted an implementation of Linear Technology's Typical Application circuit from the data sheet, minus the microcontroller and plus soft-start and other safety features.  The challenge became the layout of the PCB, on two layers, with a full silk-screen and suitable for low-cost prototype manufacturing, in an area no larger than the battery, which was 1.42 by 2.13 inches.

The battery was to be a 1.7 A.h Lithium-Ion cell, Ultralife part number UBP001, available from Mouser Electronics.  Outputs were to be the 3.3 volts at 1.0 amps, 5.0 volts at 800 mA and 1.8 volts at 400 mA shown in the data sheet's Typical Application schematic, but the 1.6 volts at 400 mA output was to be replaced with a second 3.3 volt output (all outputs can be set by resistor ratios).  Sources of power for charging were to be a USB connector and a coaxial jack for a 4.5 to 5.5 volt wall-wart.  Options of the LTC3586 were to be strapped with jumpers (replacing the microcontroller).

Switching Regulator Layout Considerations

All PCB design should be carried out by someone who understands how current flow interacts with adjacent circuit traces and the general environment, but switching power supplies are especially tricky.  This is because of the rapid changes in current path as the power inductor is alternately pumped up from the supply and drained into the load.  Fast switching is essential to reduce power dissipated by the switching components and increase the conversion efficiency.  As the intended application of the LTC3586 is in portable devices, the switching frequency is higher than usual (2.25 MHz) to minimize the physical size of the power inductors.  This makes matters worse with regard to emitted EMI.

Problems arise in both the radiation of and the susceptibility to interfering signals when circuit traces behave as antennas.  Loop antennas are formed when current flowing in a trace has to return to its source via a route that is widely separated from the outgoing path.  To prevent this, every path with a fast-switching signal must have a return path close by, either on the same layer or an adjacent layer.  This can be provided in a worry-free manner for all signals by an unbroken ground plane.  But, with a two-layer PCB required by the customer, allocating one side for a ground plane would mean that only one side is available for routing.

Component Selection

The customer required that all parts be purchased from Digi-Key, except for the battery as specified.  It turned out that the LTC3586 itself had to be obtained directly from Linear Technology.  All resistors and most capacitors were selected in the 0603 size for ease of handling.  A small reduction in PCB size would be possible using 0402 parts, but the requirement for a full silk-screen meant that a minimum area would be needed just to put down the reference designator.  Some large value capacitors were not available (or very expensive) in this size and an 0805 part was selected.  LEDs were also 0805, green for input power, yellow for charging and red for fault.  MOSFETs for soft-start control and to use in parallel with an internal switch to boost efficiency were in SOT23-3 packages.

The most difficult parts to specify were the power inductors.  It is essential that the saturation current be at least as large as the peak current flow during circuit operation under all circumstances.  For example, the 2.2 µH inductor for the 3.3 volt 1.0 amp buck/boost regulator needed to handle a peak current of at least 2.0 amps.  The LTC3586 data sheet fortunately contains an extensive applications section with all the information required.  Small physical size and high current carrying capability are opposing requirements so compromise was necessary and three of the selected inductors are as large as the power controller chip itself.

Component Placement

Whether a printed circuit can be routed or not depends not only on the ingenuity of the designer but on whether it is possible to place all the components in advantageous locations.  During placement of this circuit, it quickly became apparent that Linear Technology had considered the PCB designer in allocating pin functions to the LTC3586.  By placing the inductors around the controller, then the large capacitors and working out to the edge of the board, it was possible to arrange for relatively few traces to cross.  This, of course, was hard to see with only the "air wires" displayed, but by working steadily without breaking concentration a good placement was achieved.  Minor changes to the schematic were made when needed, for example exchanging the position of an LED and its current setting resistor.

After all the parts were placed, it was necessary to clean up the silk screen.  The customer's requirement for a full silk-screen was interpreted to mean that all parts, connections and jumpers could be identified on the finished board without reference to a separate document.  Inexpensive prototype PCB services, also required by the customer, place a lower limit on the width of silk screen lines.  It has been found that 7 mil lines usually come out well and that a character height of 40 mils is easily readable.  Within these parameters, all components were labeled.  A slightly larger character height was used for external connections to the board so as to stand out clearly.

Switching Regulator Assembled, Bottom Side


During routing, parts were nudged apart to make room for traces or moved together to close up wasted space.  The LTC3586 is a fine-pitch device, with pads spaced at 0.4 mm (15.75 mils), so 7 mil traces were used at the pads, increasing in width away from the device according to the current carried.  The required width of traces that carry high current is often overestimated.  For example, to carry one amp with a temperature rise of 10°C on an external layer of one ounce copper, a 12 mil trace is sufficient.  For this design, traces were made as wide as possible without increasing board size.  The current path from the battery, or external supply, if connected, to the regulators was implemented as a ring around the outside of the board.

Inevitably, some routes could not be completed on the top layer.  The disruptions in the ground plane on the bottom layer were made as short as possible and kept far away from the power control chip, inductors and high-value capacitors in the center of the board where large currents are switched.  All routes with bridges on the bottom layer were low current signals.


Switching Regulator Assembled, Top Side

All objectives of the design were met, except that when the batteries arrived they turned out to be a little smaller than the dimensions in the data sheet so that the PCB is a little larger than the battery.  Also, the rather bulky coaxial connector for wall-wart power extended over the edge of the board.  The customer found these results to be acceptable.  Five pieces were assembled and one extensively tested.  Results were generally in line with the LTC3586 data sheet.

Although it is not clear that the PCB will ever go into production in its present form, manufacturability was considered throughout the design.  Parts are placed in rows with consistent orientation and on a 10 mil grid so as to speed up the pick-and-place process.  In a second iteration, many parts could be squeezed closer together and/or smaller packages chosen to reduce the board size further.  A production PCB might also achieve finer lines and smaller character height on the silkscreen.