Thermal vias in an IC

[Freshman]

In this Application note recommendation for ground connection of the thermal ground pad of an IC on page 3, (https://ww1.microchip.com/downloads/aemDocuments/documents/UNG/ApplicationNotes/ApplicationNotes/AN18.15-PCB-Design-Guide-QFN-DQFN-Packages-00001843.pdf),



I see that the ground paddle of the IC, is in square shape.



So, when I place it on a PCB, it is best, if I provide the same square shape ground pad on the PCB for good thermal dissipation.



But, there's an image on page 3, bottom left, where they mention to give 16 thermal vias, 4 x 4 arrangement, and this thermal vias to ground.



My question is, why should I place ground thermal vias when I can give a proper square shaped copper ground plane? Why do I need to give vias which might be expensive that simply pouring copper?



Any advantages or reasons to go with thermal vias over square copper plane?

[mikerj]

A tiny square of copper under the IC isn't going to give you good thermal dissipation.  The idea is to thermally connect that pad (using vias) with a large ground-plane layer so the heat can be distributed over a large area of the PCB.

[aliarifat794]

A copper ground plane is beneficial for providing low impedance ground connections, reducing noise, and improving signal integrity, but its primary purpose is not thermal dissipation.
https://www.allaboutcircuits.com/technical-articles/pcb-layout-tips-and-tricks-use-a-ground-plane-whenever-possible/

[Tim S]

An alternative method more suitable for hand assembly is to put a big, single through hole pad on instead of an area with vias. Soldering is easy by poking the iron in the hole. Useful as a star point ground as well!

[wraper]

A copper ground plane is beneficial for providing low impedance ground connections, reducing noise, and improving signal integrity, but its primary purpose is not thermal dissipation.
https://www.allaboutcircuits.com/technical-articles/pcb-layout-tips-and-tricks-use-a-ground-plane-whenever-possible/

Simply not true for any SMD device that dissipates significant power.

[MarkT]

An SMT device on a multilayer board with thermal vias is better than just using a top-layer ground pour to spread heat, as there is much more metal spreading the heat laterally, and better conduction to the back side of the board too.  (And more thermal mass to handle transient loads).

For very high dissipation you may be able to use IMS with SMT parts, though you are restricted to a single layer...

[AnalogTodd]

Surface mount devices that dissipate power need to get the heat out somehow or they get too hot and die an early death. Which ways can we get power out?

• Through the plastic? You don't really get much out of the package this way. The plastic is horrible for conducting heat. The thermal resistance (much like electrical resistance, but instead of current we have power and instead of voltage we have temperature rise) is extremely high compared to other possible paths.
• Through the leads? You have plastic separating the leads from the die, otherwise you would have everything shorted to the die itself. Again, not a good way to conduct heat away.
• Through the silicon and out the backside of the package via a thermal pad? This is the best way to get heat out. It's a short path that goes through a very thin piece of silicon and then through a very low thermal resistance piece of metal. So how do we spread the heat and dissipate the power from there?

• Adding a big ground plane on the top layer. This layer is often thicker than the other layers and helps transfer a lot of heat away from the device. But remember resistance is the resistivity multiplied by length and divided by cross sectional area (thermal resistance calculates the same as standard resistance). That top layer is still pretty thin, so we need other ways to get heat out as well. The heat has to escape from as many places as possible via transfer to the environment.
• We can't go through the PCB without something that conducts the heat well. The fiberglass used for a board is usually a lousy conductor of heat, so a number of thermal vias will help get the heat through from topside to backside. Now, we can add another layer and cut the net thermal resistance to help get more heat out.
• If you add internal layers to help spread the heat as well, you can lower thermal resistance even more! You get more paths in parallel for even lower thermal resistance. If you think about it as well, the fiberglass gets thinner between the layers so it can help get heat to the other layers to dissipate it out.

Thermal management is a big thing as you get more things running in a smaller volume. Semiconductors don't like running too hot, it severely limits their lifetime and can kill their performance. I've dealt with this for years as the chips I designed would, by definition, dissipate plenty of power.

[BillyO]

Some points:

1) An exterior ground plane is much better than an internal ground plane.  They are typically both thicker and are less insulated from the ambient air.

2) For standard 1 oz. copper you don't get much more benefit from an area of more than about 1 square inch.  Beyond 2 sq. inches on a single layer there is no noticeable additional cooling.

3) It is far better to connect two external copper pours (on opposite sides of the board) of about 1 sq. in. using thermal vias than it is to have a single copper pour of 2 sq. in.

In these pictures the top pour is about 1.5 sq. in. and the bottom is 2 sq. in. and are connected with 99 vias.  This provides much better cooling than would a single plane/pour of 3.5 sq. in. and in this particular case we have about 25C per watt given free air circulation (measured).