Participate in our next Ask Me Anything about thermal management where you can ask us questions on:
• Effective thermal management strategies
• Cutting-edge technologies and materials
• Industry trends and future predictions
• And much more!
Post your thermal management questions below before June 19th and our experts @steve.carney, @allank, and @atar.mittal will get you the answers!
What are your best practices for optimizing thermal management in high density boards to ensure reliable performance and longevity?
1.What is the required area on PCB on FR4 to dissipate heat for the given power dissipation and thermal conductivity?
2.Is there a formula to calculate the required area for heat dissipation on a PCB?
1.What are the strategies to use thermal vias on LED Lighting applications?
2. Any suggestions on a thermal via pattern around LEDs for better dissipation?
This is generally application or layout specific but let me put down few points. The first thing is refer to the LED datasheet’s layout guidelines for thermal vias. Check LED package for thermal pad, if present you can add thermal vias of size 12mils hole, 24 mils pad in a grid structure or zig zag pattern. The size of the thermal pad will determine the number of vias generally 4, 5, 6 or 9. To Understand the amount of vias and their placement requires some knowledge about how much current the LED or LEDs in series, parallel combination would carry, expected heat dissipation in the region and the direction of current through the traces. Calculate the number of vias that would be necessary to carry the necessary current and double the number of calculated vias. Make use of as much copper as possible. Next step is to make sure that these vias are not clustered in a small area, make sure these vias are properly spaced and spread around the LED pad or polygon. This will not allow heat to create Hotspot at a particular area and evenly distribute the current. The most common mistake that is generally done is with the return path vias, the return path vias also should match the source end vias. The GND planes should be properly stitched using vias at multiple points to avoid thermal hotspots on the polygons, grid or zig zag pattern with 100 or 150 mils pitch will do. Similarly source polygon also can be stitched on multiple layers using vias, evenly distributed in zig zag pattern. If necessary thermal vias and thermal pads can be provided with soldermask opening for improved heat dissipation.
Here are some of the Strategies for Thermal Vias in LED Lighting
identify the hotspot or high leat dissipation components, in you case it will be high power LEDs or SMPS.
Placement of the thermal vias is very critical. place them directly underneath and around the components.
for example if you have a power ic, use thermal via like this or use differnt pattern
here are some other pattern
here is one of the eample (Image source google)
if you see the led image there is thermal pad below , if you create a pad of that shape with thermal vias specified in above pattern it will help you dissipate heat better.
Use thermal via patterns like Grid Pattern, Peripheral Ring, Central Cluster.
Connect thermal vias to large ground planes on the PCB to facilitate the spread of heat and minimize thermal resistance
use conductive or non conductive via Filling and Plating
The metal core (usually aluminum or copper) provides a direct path for heat to spread from heat-generating components,
using metal core or substrate significantly improving thermal conductivity compared to traditional FR4 PCBs.
following above techniques should provide you good heat dissipation
you can use thermal simulation tools to simulate your pcb for hotspot and identify minimum trace requirement is followed or not and also provide thermal vias to facilate heat dissipation in that areas.
if still you have heat dissipation issues use heat sinks and fans to cool
finally use our calculator this will help you calculate number via required.
please refer to my answers. i have tried covering up in detail
With high density boards, the most important is how well the stackup is planned considering the amount of traces and the number of different voltages and their current requirement. I am assuming may be a BGA is part of this board which would generally be crowded with lot of passive components and surrounded by active components. I would recommend to have at least two dedicated power planes and 4 dedicated GND planes to allow enough copper for proper heat distribution. Absolutely crucial is identifying high power circuitry and try to give them priority when it comes to placement, like your power circuitry should be planned as per the amount of current delivered in a every region and plan the placement as per the number of connections required in various region. This will allow you to plan your power plane in every region with enough copper and vias. Always fanout your components during placement itself. Never compromise on the min number of vias needed or min copper required. make sure power pins on the BGA have atleast one via per ball, do not share single via for 2 or more balls. As we know due to presence of so many vias the internal power planes will have lot of voids, therefore it is necessary to make sure the effective width of the power planes on internal layers meet the min requirements and also the current should have multiple paths to travel rather then a single path resulting in heat accumulation. Identifying the thermal conductivity of the material as per your application is also crucial, I would recommend to consult your fabricator before finalizing the PCB material. Make sure the components which are prone to lot of heat generation like BGA or power ICs are not surrounded by tall components which can block the air flow. Knowing the power dissipation of each IC, safe junction temperature and thermal resistance of every IC is important to identify whether a heat sink will be required for further heat dissipation. Plan heat sink or fan above main processors, for increased thermal dissipation, make use of thermal vias on thermal pads, soldermask openings on thermal pads can further improve heat dissipation. Increasing the metal area by connecting the GND to chassis through mounting holes will also help. Stitch GND and power planes properly with Vias to improve heat distribution.
It totally depends on your application.
suppose you have a simple power supply board with a linear voltage regulator. 5v to 3.3v drop of almost 1 volt. this will generate some heat which can be easily handled
but your application needs a cpu and gpu which will release drastic amount of heat you will need good heat dissipation techniques.
suppose your application is high power leds, there will be very high current flowing through the circuit at the same time leds its self will dissipate the lot of heat.
in led case if you use metal core in the middle. it will not solve your problem as entire pcb will get hot, it will try to dissipate heat across the surface area of the pcb but. it will be not enough.
on top if you pcb is enclose in some container/BOX, surrounding air will heat up that will raise the temperature further.
ideal solution to the LED boards are usually lot of themal via with via filling and plating, use usuallu 2 layer boards with metal substrate (slightly costly) or use thermal tapes/adhesive to metal fixtures to externally dissipate heat. also using fans to blow air will help.
now coming to your query
when internal space is limited metal core pcb will help you dissipate heat evenly accross the entire pcb providing better heat dissipation compared to FR4.
but there is a limitaion to it how much heat that can be dissipated, if you have close container and no place for air flow or any other metal surface to cool off, sounding environment will heat up which will raise the temperature of components and cycle will continue till something breaks.
now if you concern with heavy metal parts you may have to go for light weight material, since its a tight space putting a fans or liquid cooler is not an option then you have to totally rely on best layout practice, good material, better chassis.
1. I understand it’s a complex issue, but is there a potential future where we can eliminate metal chassis components in mobile and IoT devices to reduce product weight?
this will be difficult as IOT and mobile are opting for higher processing power. more the processing more heat will be generated by the cpu and gpu. also supporting components.
for example if you see mabook air m3 (not promoting any brands here) works without fan even with GPU. the metal casing act as a heat dissipator, since the entire frame is of high quality light weight material it can dissipate a lot of heat quickly to larger surface area. which cools the gpu/cpu very quickly. also metal
This is not so straight forward, calculating the amount of area for a given power dissipation is tricky, since the heat dissipation is due to various principles such as convection, conduction and radiation. Generally the power dissipated in various ICs results in heat generation, therefore the heat is actually generating around the IC and sometimes simply increasing the copper would not be helpful, yes it does help in distributing heat but that depends on whether the IC will be able to hold on to safe junction temperature until the heat is distributed. Knowing the Thermal resistance of the PCB material and various thermal resistances associated with the IC packages such as Junction to Ambient, Junction to thermal pad are crucial in identifying the correct junction temperature. The best thing to do is read the datasheet for any thermal guidelines provided when it comes to high power ICs and try to replicate the same without any compromises. Increasing the copper thickness will further improve the thermal characteristics. I found a good reference for you to properly understand in detail how all this works which also provides few formulas and thumb rules. https://www.ti.com/lit/an/snva419c/snva419c.pdf
