Thermal Management Design Using Insulated Metal PCBs or Metal-Clad PCBs
Editor's Note: This article is from Chapter 2 of the eBook "The Printed Circuit Designer's Guide to...Thermal Management: A Fabricator's Perspective" authored by Anaya Vardya, CEO, American Standard Circuits, and published on iConnect007 here.
Insulated metal PCBs (IMPCB) or metal-clad PCBs (MCPCB) are a thermal management design that utilizes a layer of solid metal to dissipate the heat generated by the various components on the PCBs. When metal is attached to a PCB, the bonding material can either be thermally conductive but electrically isolative (IMPCBs or MCPCBs), or in the case of RF/micro- wave circuits, the bonding material may be both electrically and thermally conductive. The reason that RF designers usually have the bonding material thermally and electrically conductive is that they are using this not only as a heat sink but also as part of the ground layer. The design considerations are quite different for these different applications.
This chapter will focus on the IMPCB design considerations, and Chapter 4 will focus on RF thermal management. We will focus on things designers should be discussing with their PCB supplier to ensure manufacturability and a successful product launch. Since the choices, options, and decisions can be extremely complicated, it is critical to engage early and collaborate with the PCB fabricator about the specific design to ensure the most cost- effective solution.
Some of the more common applications of IMPCBs include:
Power Conversion: Thermal-clad offers a variety of thermal performances, is compatible with mechanical fasteners, and is highly reliable
LEDs: Using thermal-clad PCBs ensures the lowest possible operating temperatures and maximum brightness, color, and life
Photovoltaic Energy: Renewable energy to power telecommunications, military camps, residential and commercial structures, and battery charging stations
Motor Drives: Thermal-clad dielectric choices provide the electrical isolation needed to meet operating parameters and safety agency test requirements
Solid-State Relays: Thermal-clad offers a very thermally efficient and mechanically robust substrate
Automotive: The automotive industry uses thermal-clad boards, as they need long term reliability under high operating temperatures coupled with their requirement of effective space utilization
IMPCB Benefits
- Excellent surface mount cooling
- High electrical isolation, insulation, and thermal dissipation
- Low cost
- Robust thermal performance
- Thermal conductivity of the dielectric in the range of 0.6–8 W/mK
- Manufacturability (integrates with standard PCB processing)
Thermal Properties Explained
A thorough understanding of a number of different thermal properties is needed to be able to design the appropriate IMPCB solution to a thermal condition, including thermal conductivity, thermal impedance, and thermal resistance.
Thermal Conductivity
Measurement of the ability of a substance to conduct heat (W/mK)
A material property, meaning that it does not change when the dimensions of the material change, as long as it is made up uniforml. For example, the thermal conductivity of 1 cm3 of gold is exactly the same as the thermal conductivity of a 100 m3 of gold
Generally obtained in the industry using one of two tests: The D-5470 test, or the E-1461 standard ASTM tests
The D-5470 test measures the thermal impedance in Kcm2/W of the sample and determines the thermal conductivity through the following relation:
Thermal conductivity = Thermal diffusivity * Specific heat capacity * Density
Thermal Impedance
- This is the opposite of thermal conductivity. It is a measurement of the ability of a material to oppose the flow of heat, so from a PCB point of view, we want this value to be low. The lower the thermal impedance, the quicker heat flows through the PCB and to the heat sink where it is dissipated
- Its value depends on the thermal conductivity of the material and its thickness; in other words, this is not a material property, but is an object property, as changing the thickness of the material will change this value. However, changing the area of the material will not change this value (as long as the thickness stays constant)
- For example, the thermal impedance of a sheet of laminate is the same as the thermal impedance of a cut piece of the laminate, say 1 cm2 of it. Whereas the thermal impedance of a sheet of gold of 1-mm thickness is different from the thermal impedance of a sheet of 2-mm thickness
- This is generally obtained using the D-5470 test mentioned above and relates to the thermal conductivity via the following relation:
Thermal impedance = Thickness / Thermal conductivity
Thermal Resistance
- Thermal resistance (measured in K/W) is basically the same as the thermal impedance. The difference is that it takes into account the area of the sample as well as the thickness and conductivity
- Changing either the thickness, or the area of the material, will change the associated value of the thermal resistance as follows:
Thermal resistance = Thickness / (Thermal conductivity * Sample area)
Single-Sided IMPCBs
In its simplest form, an IMPCB is a piece of copper foil that is bonded to a thermally conductive dielectric and a metal substrate (Figure 2-1). Typi- cally, a PCB supplier can buy the copper foil laminated to the base metal from several different laminate manufacturers. A laminate selector guide is provided in Appendix B.
Some of the key design factors to consider include the following.
Copper Thickness
Typically ranging from 1–6 ounces with 1 and 2 ounces being the most commonly used. The thicker the copper, the more expensive the cost of the PCB.
Thermally Conductive Prepreg
This is one of the most important elements of this construction and what typically differentiates the various suppliers. This is the substance that both electrically isolates the copper circuitry from the main metal and helps with the rapid transfer of heat between the two. It ensures that heat generated by the components is dispersed to the base metal (heat sink) as quickly as possible. The prepreg is typically an organic resin with ceramic fillers to increase thermal conductivity. The filler type, size, shape, and percentage are some of the factors that determine the thermal conductivity performance. The usual ceramic fillers are Al2O3, AlN, BN, etc.
The performance of the various prepregs is measured by the thermal conductivity (W/mK) and thermal impedance (Km2/W). The higher the thermal conductivity, the better the heat transfer, and the lower the thermal impedance, the better the heat transfer. However, it is also important to understand that the better the heat transfer associated with the prepreg, the greater the cost. Therefore, it is critical not to over-design. To put this in perspective, the thermal conductivity of FR-4 is approximately 0.2–.4 W/mK, whereas the thermally conductive prepregs that are available on the market today range from 1–7 W/mK. Apart from thermal conductivity, the thickness of the dielectric can be critical. Typically, the thickness of the dielectric ranges between 2–6 mils, with 3-mil dielectric as the most common.
Base Metal
Aluminum is the most common base metal used. The two most common types are 5052H32 and 6061T6. 5052H32 is typically less expensive and a lot more available than 6061T6. The thickness of the aluminum typically ranges between 40–120 mils, but 40 and 60 mils are the most common thicknesses available.
Table 2-1: Properties of various base metals.
There are also cases where copper is used as a base metal. Copper is some- times used for better thermal conductivity, mechanical strength, and CTE match to thicker copper foils. In most applications, the thermal advantages of the copper base plate are insignificant because the thermal resistance of the base metal is small relative to the thermal resistance of the dielectric layers and the components. This is a significantly more costly solution, as well as significantly heavier. A brief comparison of the various base metals is illustrated in Table 2-1.
Maximum Operating Temperature
Work with your PCB fabricator and raw material supplier to ensure that the MOT you require is being met by the material selected.
Breakdown Voltage
Ensure that you understand the voltage at which the material dielectric will breakdown and short the circuit. As a general rule, the thinner the dielectric, the lower this value will be.
Panel Utilization
The IMPCB laminate materials are significantly more expensive than FR-materials. As a ballpark, a 0.062” IMPCB material may be three times more expensive than an 0.062” FR-4 material. It is, therefore, extremely important to understand how the board/array designs utilize the production panel. This is another area where early engagement with the PCB supplier is important. The most popular size for a working panel on these materials tends to be 18” x 24.” As many PCBs are processed as arrays, it is critical to ensure that array designs are such that panel utilization is maximized. Many large PCBs may be processed without rails through the assembly operation due to the rigidity of the material. This can vastly help improve panel utilization.
Machining/Fabrication
Scoring is the most common process used for square or rectangular shapes. The advantage of scoring is that it assists in maximizing material utilization since zero spacing is needed between parts to score them. In contrast, routing is the most expensive process since it is slower and requires spacing between parts and will likely reduce material utilization. Make sure that the PCB fabricator has a scoring system that is specifically designed for scoring aluminum. The scoring machine should be equipped with a lubrication system. It is recommended to use diamond-coated scoring blades and router bits when dealing with aluminum base metal.
Solder Mask
There are many single-sided IMPCB designs that are used for LED lighting applications. A majority of these applications require white solder mask. Thus, it is important to address this as all white solder masks are not made equal. A lot of LED customers are looking for consistency in the color of their white solder mask. The marketplace today has several different solder masks that are marketed as LED solder masks.
Figure 2-2: Different colors on two different types of solder mask.
The issue is that they visually look different when you put them side by side. Some solder masks have a “bluish” hue to them, and others have a “yellowish” hue (Figure 2-2). Also, the colors look different with one coat vs. two coats of solder mask, so this is another decision that will need to be made. Another consideration is that there can be an interaction between the surface finish, the solder mask, and subsequent heat processing steps in the assembly process. Some solder masks tend to change colors more than others with additional heat.
Figure 2-3: Solder mask “browning” with multiple reflows.
Boards with lead-free hot air solder leveling (HASL) tend to become “yellower” the more heat they are subjected to. We have stopped reworking boards through lead-free HASL (only one pass is allowed). Figure 2-3 illustrates the same solder mask after lead-free HASL vs. a board that has been through two assembly reflow cycles.
Boards with ENIG after the solder mask process may get “pink” with subsequent reflow. The reason for this is that “dirty” rinses in the ENIG process with gold residue form a complex with the titanium pigment in the solder mask which then turns the solder mask purple in the high-temperature assembly process. Thus, it is important for the PCB supplier to manage the rinses on the ENIG bath very carefully (Figure 2-4).
Figure 2-4: “Pinking” solder mask on an ENIG board with multiple reflow cycles.
Manufacturing Process for Single-Sided IMPCB
The manufacturing process for single-sided IMPCBs is illustrated in Figure 2-5.
Figure 2-5: Single-sided IMPCB process flowchart.
Pedestal Technology
For LED applications with a demanding heat transfer profile, inte- grating pedestal technology may be the optimal solution. The pedestal construction on metal-core PCBs allows the designer to get a direct path between the LED (heat generator) and the metal core of the PCB. A typical LED is soldered to a copper pad and the heat must transfer through the PCB dielectric material before it gets to the metal core.
Figure 2-6: LED pedestal construction.
Another option is to use thermal vias to get a more direct transfer to the metal core. Both of these designs are suited for lower-heat applications but may not be optimum for high-heat generators. A pedestal is simply a buildup of copper plating from the metal core up to the surface of the PCB. Thermal conductivity of up to 400 W/mK can be achieved using pedestal technology if the metal core is copper. The cross-section view in Figure 2-6 visually highlights the “pedestal” effect of this construction.
Figure 2-7: Double-sided IMPCB.
Double-Sided/Multilayer IMPCB
The PCB supplier manufactures a double-sided or multilayer IMPCB and then bonds it, utilizing a thermally conductive prepreg to metal (Figure 2-7). The bonding process is done in the same multilayer press that is used to manufacture a multilayer PCB. A lot of the design factor considerations discussed in the single-sided IMPCB section apply to double-sided as well. Some additional considerations to think about include the following.
Copper Weights on All Layers
The thicker the copper, the more expensive, and remember that the outer two layers will get additional copper since the vias will need to be plated. Lines and spaces should follow the design guidelines of the PCB fabricator based on the copper weights of each of the layers.
Double-Sided/Multilayer Construction
It is important to decide whether you can use FR-4 for your multilayer construction or if you require thermally conductive prepregs and cores. If you need thermally conductive cores and prepregs, there are a number of options available, but core thicknesses are limited, so it is best to work with the PCB fabricator or laminate supplier on constructions that would make sense. The prepregs tend to be low flow, so it is important to work with a PCB fabricator that understands the press cycles and flow dynamics of the specialty prepreg that need to be used.
Thermally Conductive Prepreg
Choose the prepreg to bond the PCB (double-sided or multilayer) to the metal based on thermal conductivity required and thickness of the copper circuitry. From a PCB manufacturing perspective, several different factors need to be taken into account for in the process of bonding the PCB to base metal:
- Ensure that you don’t have delamination between the PCB and the metal. There are design factors that can impact this and process conditions in the lamination process
- Have a method to control the flow of the prepreg through the plated through-holes (PTHs) to the top side, and then have a method to remove any flow that ended up on the top surface of the PCB
- There are a number of mismatched CTEs in this package. It is important to balance the copper in the construction as much as possible from a PCB perspective and have a press cycle that minimizes warpage
Base Metal
Aluminum is the most common; however, there are many applications that will also use copper as the base metal. In general, for this kind of construction, if aluminum is the metal of choice, I recommend using the 6061T6 alloy.
Manufacturing Process for Double-Sided/Multilayer IMPCB
The manufacturing processes for double-sided and multilayer IMPCB are illustrated in Figures 2-8 and 2-9. The processes are similar to double-sided and multilayer PCBs described in detail in our book Fundamentals of Printed Circuit Board Technologies (more books listed in our further reading section).
Figure 2-8: Double-sided IMPCB process flowchart.
There are two major differences. First, when one utilizes the thermally conductive prepregs, the press cycles need to be well-defined due to the low-flow nature of the prepreg. Second, there is an additional press cycle since after the board is completed, one need to bond the PCB to the aluminum. The aluminum prep before bonding and the press cycle associated with the bonding are critical.
IMPCB Testing Methods
This is a bit of a caveat emptor (buyer beware) caution regarding the testing of IMPCBs, particularly when the PCB fabricator is in China or otherwise outside of the U.S. There are a few factors to be considered:
- Datasheets provide several different ways that laminate suppliers can test these materials for thermal conductivity, and to date, there are no IPC standards for this. A thorough understanding of the test methods utilized is required since all materials advertised as 2 W/mK may not result in similar performance (Appendix A describes the various test methods)
- Some laminate suppliers 100% HiPot test their materials, others will test them if you request it at an extra cost, and many don’t have the ability to test their material
- There are many suppliers that can supply single-sided IMPCB materials, but the supply base is quite limited for multilayer cores with high thermally conductive prepreg and thermally conductive prepreg that can be used to bond the multilayer PCBs to the metal
Figure 2-9: Multilayer IMPCB process flowchart.
IMPCB Fabricator Selection Considerations
The supply base for IMPCB suppliers is relatively small, which makes the supplier selection a critical task. Some of the things to consider include the following suggestions:
- The fabricator's experience with manufacturing IMPCB materials
- A fabricator that has manufactured a variety of different types of IMPCBs and materials from a variety of material suppliers
- A fabricator that has a good relationship with the material suppliers in the space
- The fabricator is willing to work in partnership with you keeping an open mind when it comes to your ultimate needs
- If UL is important to your application, ensure that the fabricator has the requisite UL listing(s)
- A fabricator that has the process controls and disciplines in place to consistently meet all your requirements
- Lead-times vary between different fabricators, which is compounded when procuring from a source outside the U.S. If you are interested in multiple regions, choose a fabricator that has a support structure in all regions of the world (supply chain ease)
- Another important factor could be R&D that is being done by the laminate supplier that may support future technology. As an example, there are a couple of laminate suppliers that have developed special laminate materials where the aluminum can be bent/formed without compromising the copper circuitry or the dielectric layer