Technical Information Site of Power Supply Design

FAQ   Design Support Tools   - 繁體中文   - 简体中文   - Japanese

2021.02.24 DC/DC

Inductor Placement

PCB Layout of a Step-Up DC/DC Converter

In the previous article, placement of output capacitors and freewheel diodes was explained. In this article, we explain the positioning of inductors, which are next placed on a board.

Inductor Placement

After output capacitor and freewheel diode placement, the inductor is positioned.

The inductor L is placed near the switching MOSFET Q2 in order to minimize radiated emission from the switching node. The area of the wiring copper foil should not be increased beyond what is necessary. One way to lower the wiring resistance and improve heat dissipation from the copper foil is to expand the copper foil area, but if the foil area is too large, it acts as an antenna and may cause increased EMI.

One guideline to use when determining wiring widths, after having considered the wiring resistance, heat dissipation, and antenna effects, is current rating. The following graphs indicate the temperature increase due to the current being passed and the conductor width. For example, when a 2 A current is passed through wiring with a conductor thickness of 35 μm, if the temperature increase is to be held to within 20°C, then the Δt=20°C curve (light blue) is referenced to determine the wiring width at 2 A. In this case, we find that a conductor width of 0.53 mm is sufficient.

In actuality, because wiring is affected by heat generated by nearby components and the ambient temperature, it is recommended that the conductor width be selected with ample margin included. For example, for a one-ounce (35 μm) board, the conductor width is generally set to 1 mm or more per ampere of current, and for a two-ounce (70 μm) board, the width is generally made 0.7 mm or more per ampere. In this way, separate design rules that include margins are typically applied.

Below are shown a layout example in which wiring area is optimized from the standpoint of EMI, and a poor layout example in which the wiring area is made larger than necessary. The layout sections being discussed are shown in a darker color.

Where inductor wiring is concerned, there are two other points to be noted. The first is that the ground layer must not be located directly below the inductor. Due to the effect of cancelling magnetic lines of force caused by eddy currents occurring in the ground layer, the inductance of the inductor L drops and losses increase (reduced Q) (see the left side of the diagram below). Apart from the ground layer, switching noise can propagate in signal lines as a result of eddy currents. Hence wiring should never be located directly below the inductor. When wiring below the inductor cannot be avoided, an inductor with a closed magnetic circuit structure and little leakage of magnetic lines of force should be used.

The second point to note is the distance between inductor terminals. As in the example on the right in the diagram above, because the copper foil area is broader in the terminal portions, the effective distance between the terminals is reduced, and the high-frequency signal of the switching node may be induced in the input via stray capacitance. As with the other wiring examples, the copper foil for the inductor terminals should be limited to the minimum amount necessary.

Key Points:

・The inductor should be placed close to the switching MOSFET Q2, and the area of the copper foil wiring should not be made larger than necessary.

・As a guideline for determining the wiring width, the current rating should be considered, and the width should be chosen with a margin included.

・The ground layer must not be located directly below the inductor. In addition to the ground layer, signal lines should likewise not be positioned below the inductor.

・If wiring directly below the inductor cannot be avoided, an inductor with a closed magnetic circuit structure and minimal leakage of magnetic lines of force should be used.

・The distance between inductor terminals should not be shortened.

PCB Layout and Selection of Peripheral Parts

This website uses cookies.

 

By continuing to browse this website without changing your web-browser cookie settings, you are agreeing to our use of cookies.