DC/DC Converter PCB Layout
Placement of Thermal Vias
In succession to the preceding discussion of "Placement of Input Capacitors and Output Diodes", we now turn to "Placement of Thermal Vias".
- Current Paths During Step-Down Converter Operation
- Ringing at switching nodes
- Placement of input capacitors and output diodes
- Placement of thermal vias
- Placement of inductors
- Placement of output capacitors
- Feedback path wiring
- Resistance and inductance of copper foil
- Via resistance, inductance, allowable current
- Noise countermeasures: corner wiring, conduction radiation
- Noise countermeasures: snubber, boot resistor, gate resistor
The use of thermal vias is well known as a method that uses the circuit board to improve the heat dissipation of surface-mount components. Structurally, a penetrating hole is opened in the board, and if the board is a double-sided board with a single layer, copper foil is used to connect the board top and bottom surfaces, in order to increase the area and volume used for heat dissipation, that is, to lower the thermal resistance. In the case of a multilayer board, thermal vias may connect multiple layers, or may be limited to only partial connection of layers, but in all cases the basic principle is the same.
Surface-mount components assume that by mounting on a PCB (printed circuit board), thermal resistance is reduced. Thermal resistance depends on the area and thickness of the copper foil on the PCB that serves to dissipate heat, as well as on the thickness and material of the board. In essence, the broader and thicker these materials, the greater is the effect in dissipating heat; but the thickness of the copper foil generally conforms to standard specifications, and cannot be made unreasonably thick. Moreover, given that miniaturization continues to be a basic design requirement, the PCB area cannot be made as large as one would want, and the thickness of the actual copper foil cannot be described as very great either, so that when a certain area is exceeded, a heat-dissipating effect commensurate with the board area cannot be obtained.
One measure in answer to these issues is the use of thermal vias. In order to effectively use thermal vias, it is important that the thermal vias be located close to heating elements, for example, directly below components. As indicated in the diagram below, the effect of thermal equilibrium is utilized, and so it should be apparent that connecting areas with large temperature differences is a good plan.
Placement of Thermal Vias
From this point we explain actual layout examples. The following diagram is an example of the layout and dimensions of thermal vias for an HTSOP-J8 package, a package type in which a heat-dissipating plate is exposed on the bottom surface.
It is recommended that the thermal vias have a small inner diameter of approximately 0.3 mm for filling by plating, in order to heighten thermal conductivity. If the hole diameter is too large, problems with solder suction may occur during the reflow soldering process, so due caution is necessary.
With the interval between thermal vias set to about 1.2 mm, the vias are placed directly below the heat-dissipating plate on the bottom surface of the package. In cases where heat dissipation is insufficient using only vias directly below the bottom heat-dissipating plate, thermal vias are also placed on the periphery of the IC. In this case also, it is important that the vias be positioned as close to the IC as possible.
The placement and size of thermal vias and other parameters will probably differ depending on the expertise at different companies, and may be formulated as rules. In such cases, the above remarks should be born in mind when studying how best to achieve satisfactory heat dissipation.
・Thermal vias are a means for causing heat to be conducted through a passage (hole) penetrating a circuit board to the opposite side, where it is dissipated.
・Thermal vias are placed directly below heating elements, or as close to them as possible.