Catharina R. Biber, Wakefield Engineering Inc.

Abstract

This article describes how Computational Fluid Dynamics (CFD) can help in the selection and/or design of a heat sink for electronics cooling applications. CFD modeling complements the other tools in the thermal tool kit: calculations based on approximations and correlations; and experimental work. Whether the application includes single or multiple heat sinks, the visualization power of CFD can help users to make better, faster design decisions than is possible using traditional methods.

Introduction

The performance of any heat sink is measured by the temperature difference between its base and the local ambient, normalized to the dissipated power. This performance is a strong function of the operating environment. Accurate knowledge of the fluid (air) flow and temperature distribution around the heat sink is necessary to calculate the heat sink performance. When the heat sink is operating inside a populated enclosure, it is not, in general, possible to estimate the fluid velocity and temperature with a reasonable degree of confidence. This is where Engineers can gain the greatest benefit by using CFD. CFD provides a visual and numerical description of the flow field and temperature distribution in and around the heat sink inside the enclosure.

Step 1: System Level Calculations

Before beginning the modeling process, it is important to identify the goals and the scope of the proposed analysis. Generally, the objective is to select the best of several designs, and to determine the air flow distribution in the system.

The air flow, after all, is what carries the heat away from the component; the heat sink just makes that process more efficient. In order to prevent the model from becoming too large and requiring large computing resources, it is important to limit the scope of each model to a tractable size. At this stage the Engineer needs to get a good idea of the air velocity and air temperature throughout the cabinet.

There are several important pieces of information the Engineer will need before starting on the system model. He/she must know the general configuration of the system, vent locations, fan size, its location and its performance curve. A system model must include any large blockages to the flow: power supplies, cables, connectors, cards, EMI filters and similar items. Smaller obstructions must be omitted or combined together into an average component height or a larger object with equivalent area.

The primary objective of this phase of the work is to obtain the local air velocity and temperature upstream of the heat sink. In order to do that, the system resistance must be reasonably well modeled, so that the fan pulls the right volume flow rate. If the system air flow must maneuver around baffles and obstructions, details of the heat sink should be omitted, or a combined representation of the heat sink used. When developing the component model, the Engineer should use the air flow well upstream as the flow boundary condition. If the heat sink is likely to be the dominant obstruction, as for a high power dissipation heat sink, he/she will need to make some assumptions about it and include a schematic representation of it in the system model. It could, for example, simply be modeled as a flow resistance.

The velocity and temperature distribution in the system model can be predicted without modeling many components in detail. An example of this approach would be to include air flow passages and vents, and distribute the power dissipation uniformly. It is important to include any features that would restrict air motion around the heat sink. It is also necessary to include any power sources that would preheat air, and induce motion, around the heat sink. In passively cooled systems, CFD is even more valuable on account of its power to handle the coupling between the momentum and energy equations. It is important to note that there may be time dependent phenomena which could keep a steady-state model from converging.

Step 2. Heat Sink Design

The most efficient way to design a heat sink is to perform an analysis based on fully-developed flow correlations. Although the flow is not necessarily fully-developed, as a design strategy it is easier to make that assumption. The CFD modeling the Engineer will do later will show exactly how the flow is behaving around the heat sink. Fully-developed flow analysis will follow the same general trends, and in many applications, manufacturing constraints on the heat sink will limit the extent to which its performance can be improved. For an extruded heat sink, the fins are very efficient. It is sufficient then to use an average fin thickness for tapered fins.

To start the design, a reasonable expected value for the velocity between the fins based on the air flow boundary conditions should be chosen. A geometry based on typical manufacturing values should be used; these can be obtained from vendor catalogs, or from Table 1.

The heat sink should be analyzed as a straight flow through straight, continuous fins. Applicable correlations for forced convection, fully developed laminar flow in rectangular ducts are given in White, 1991. A good source for correlations applying to natural convection is Guyer, 1989. Pin fins can be approximated quite well as continuous fins, unless the flow is angled relative to the channel direction. In practice, the performance of dense rectangular pin fins is usually within 10% of a straight fin heat sink.

Step 3. Heat Sink Model

Once the Engineer has a general idea of the heat sink parameters design, and local air flow boundary conditions, he/she can build the heat sink detailed model. Some strategies to minimize the amount of work are to use symmetry wherever possible; to use whatever heat sink model building capabilities is offered by the software; and to represent the heat dissipation area on the base of the heat sink by a simple heat source.

Important areas to model are the fluid flow area near the heat sink surfaces and the approach areas. In the approach areas the Engineer needs to know what the flow behavior is, so it is important to model all the fluid around the heat sink, all the way to the nearest obstructions. Between the fins, or in any air spaces, the Engineer will need the velocity profiles to show the proper flow behavior. Usually three cells are adequate for showing the correct trends for laminar flow between surfaces.

Inside the solid material of the heat sink, one cell is usually sufficient in the fin thickness direction. At least four cells should be allowed for in the fin height direction to account for temperature difference along the fin height. For a very small source, at least three cells of approximately the same size as the source should be allowed in the plane of the heat sink near the source. At least two cells should be used in the base thickness. These numbers must be modified to ensure that the results given by the CFD software are sufficiently independent of the grid choice.

Now that the heat sink has been modeled in CFD, the temperature distribution can be readily obtained. Problems to look for are areas of large temperature gradient within the solid, indicating that the heat sink is too thin; sections where the air temperature is close to the fin temperature (typically towards the back of the heat sink). This is caused by the air that may flow up and out of the heat sink; and cool fins, indicating that they are too far away from the heat source to have any effect. The combination of the temperature distribution and the air flow distribution will help the Engineer to decide what design changes may be necessary in order to achieve the heat sink performance goals. The heat sink design then becomes an iterative process.

Now the process becomes iterative for the selection of the most promising heat sink design. To understand its effect on the device junction temperature, the Engineer may then need to model the component and the interface material as well as the surrounding board. This model will allow him/her to determine the maximum chip or junction temperature, which is, after all, the goal of the whole exercise. When modeling the whole system, the interface resistance between the component case and the heat sink should be included. Interface material vendors supply this information typically as a resistivity, the resistance normalized to the area. For advice on component modeling, consult the software or component vendor. They may have ready-made models you can use to speed up the process. To model the heat spreading ability of the board, the Engineer must concentrate on the power plane layers in the plane of the board, since they usually dominate. If most of the air flow in contact with the board is on the side opposite the component and heat sink, the Engineer will need to account for the thermal conductivity of the epoxy-glass layers as well.

Step 4. Verification

The next step is to verify the design experimentally by measuring the base temperature relative to the local air temperature. It is important to ensure that the measurement devices are in good thermal contact with the heat sink; an electrical continuity check assures at least some thermal contact. It is also important to get an accurate value of the power being dissipated through the heat sink. Errors can be minimized by using a heater well insulated on the back side, and by taking voltage measurements as close to the heater as possible.

The Engineer should not be alarmed if the numerical results do not exactly match the measurements. The heat sink model was just a model. The experimental prototype is also a model. The true performance of the heat sink is at best bracketed by the errors inherent in both measuring and modeling. Also, the CFD model gives only an average temperature of a grid cell, whereas an experimental measurement is really the temperature of the sensor that has been installed to make the measurement. In the final analysis, the goal of the CFD work is to make a good design decision, and as long as the Engineer has represented the physics of the problem correctly, the trends will be correct.

Summary

In order to use the power of CFD in the heat sink design process, it is necessary to model the surrounding system adequately. Air flow path configurations are as important as heat flow path details. Once the heat sink is modeled, viewing the results helps to suggest effective design changes. Experimental validation provides valuable feedback on modeling. Even if the agreement between physical models and numerical models is not perfect, model performance trends should be represented well enough to shorten the total design cycle.

Catharina R. Biber, Ph.D.
Wakefield Engineering, Inc. 60 Audubon Road, Wakefield, MA 01880, USA
Tel.: +1 (617) 224 3560 Fax: +1 (617) 246 0874
Email: cbiber@wakefield.com

References
Guyer, E., editor, Handbook of Applied Thermal Design, McGraw-Hill, 1989. White, F. M., Heat and Mass Transfer, Addison-Wesley, 1991.

Web page conversion/development by InfoVision Technologies, Inc.
sales@ivtinc.com