Should thermal vias have annular rings, should use thermal relief or direct connect?

Thread Starter


Joined May 22, 2019
Hi all, few questions about thermal vias for dissipating heat to a large copper area below a SiC Schottky diode.

In a previous design I used 0.3mm vias spaced apart 0.8mm, with no annular ring and direct connect. The dissipation was quite a bit more than I expected.

I am redesigning the board and revisiting the topic of thermal management using vias. I am unsure whether my thermal vias should have any kind of annular ring or just be a 0.3mm copper plated hole. I am working with the assumption that annular rings are for a good connection to a copper trace, but I am not so sure whether that matters if a 0.3mm is directly connected to a large copper plane, and whether any annular ring would improve thermal impedance or solderability. Some resources such as state that to avoid breakout, annular rings should be >8mil, but again this does not directly refer to thermal vias connecting to a large copper area on a different layer. I currently have a via that is 0.3mm in diameter, with a minimum 8mil (0.2032mm) annular ring, which looks like this:


References online typically are not clear on this - and often the vias don't seem to have any annular rings from photos that I have seen. But to understand the effect on thermal impedance could be interesting....



Joined Jan 27, 2019
It stands to reason that a via in a flood is akin to an effectively infinite annular ring. I can’t see any logical reason an annular ring, effectively cut into the flood, would improve anything. You would be reducing the area available for thermal conducting to the ring, with the PCB dating as a thermal insulator between it and the rest of the copper that would otherwise be connected.

I can’t be certain but.I would be mightily surprised if there is some kind of counterintuitive reason an annular ring in your case would be any kind of improvement in thermal conductivity. The fact that your intuition suggests it will improve solderability is should also indicate it reduces the thermal mass connected to the via since solderability in floods is reduced by heat dissapation.

So, my decidedly non-expert opinion is that you’d want the maximum copper area connected to your via for thermal conductivity.


Joined Jun 8, 2013
I don't see why an annular ring is needed. The part will need as much copper area contact as possible for electrical current transfer below the part. So an array of thermal vias, in a sold isolated copper plane below the part, make more sense as the heat would be transferred thu the via to the copper on the opposite side of the PCB. If the part is mounted on a heat sink, then no thermal vias would be needed.

Just my opinion..

Thread Starter


Joined May 22, 2019
Thermal reliefs on PCB layouts are for the soldering process, not for heat sinking properties. In fact it is just the opposite.
It is to allow the pad or via to reach temperature for solder to flow and create a good electrical bond.
That makes sense. So not worthwhile using on such a SiC diode with a heat sunk pad? How do you ensure good solderability without thermal reliefs,and not have a large thermal impedance and thus the part getting overly hotter than expected?


Joined Oct 2, 2009
That makes sense. So not worthwhile using on such a SiC diode with a heat sunk pad? How do you ensure good solderability without thermal reliefs,and not have a large thermal impedance and thus the part getting overly hotter than expected?
So the two are opposing properties. Which one is more important to you?
If you want heat sinking capabilities, then don't use thermal relief. When soldering the component use a higher wattage soldering iron.


Joined Oct 7, 2019
In our factories they heat up the entire board when soldering. We did tests and there is no reason for thermals. When you hand repair a board there might be a problem heating up the part. I do not use thermals relief when I solder via hot air. Most of the time I use a hand solder iron and don't have a problem. (just know it takes more energy)

Most of my projects combine high voltage and high current and hot parts. I do have a "hot plate" to warm up the board before hand soldering but I have never used it.

Jon Chandler

Joined Jun 12, 2008
Yes, a via should have an annular ring. It's what anchors the copper in the hole. What happens to this ring when stitching fill layers together? It's incorporated into the layers. In this case, is there a practical difference in specifying an annular ring vs not? Probably not. But specifying no ring may generate errors when the fab house checks the files and needless emails about what you're trying to accomplish. It's also possible it might cause errors in the copper layer.

The picture below shows the difference between a pad and a via stitching layers together. From the point of view of the copper, there's no difference. The annular ring dimension only affects the soldermask. For the pad, there's a hole in the soldermask, exposing the annular ring area copper for plating and for eventual soldering of a component lead.

pad vs via.jpg


Joined Apr 3, 2014
Thermal pads for components are designed to conduct heat away from the component. To do so efficiently vias should not have thermal spokes or any sort of isolated or disconnected annular ring. This will likely make the part hard to solder by hand but will have minimal or no effect at all on an automated reflow soldering system, i.e. systems used by PC board assembly houses.


Joined Mar 30, 2022
As said so well before me - the thermal pads serve to convey heat out of the via. When the need is to prevent component overheating, they are useful, but when we want to solder the component - they are a menace, since we cannot get the land temperature up. Heating the whole board is not so healthy, keeping in mind that behind all those fancy words - the board is made essentially of plastic and suffers high thermal expansions, which in turn exercise high tensile force on the PTH copper.
One possibility for the design of thermal vias that I can offer you is something like that (excuse my poor drawing abilities):
This way you are keeping the innerlayer lands that help anchoring the PTH, connect the land to the copper-plane, but reduce the area crossection for heat flow.