Comments on Thermal Relief – Yes or No?
Parent
Thermal Relief – Yes or No?
In my PCB design, I have 0402 components connected to polygons. To reduce the risk of tombstoning, I connected them using thermal relief.
My guiding principle is that if heat dissipation is not symmetrical on both sides of the component, and the component is 0603 or smaller, thermal relief should be applied. I differentiate between three cases:
-
Both pads are connected to polygons. (See Image 1: C14, C15, C16, C17)
-
Only one pad is connected to a polygon. (See Image 2: R10)
-
Neither pad is connected to a polygon. (See Image 2: C12, R11)
In the third case, I made an effort to route the traces symmetrically to the component to ensure even heat distribution. This follows recommendations I found online to prevent tombstoning—see Image 3.
Another consideration is whether the components will be soldered or desoldered manually, such as jumpers.
Additionally, I assume that for TH components, thermal relief should always be used when they are connected to a plane/polygon.
My Questions:
-
Are my assumptions correct? Should thermal relief be applied/not applied in each of these cases?
-
If thermal relief is used for thermal reasons, is it important that the number of connections (or their total width) be symmetrical?
-
When considering symmetry, should factors like polygon size, nearby vias, and other thermal paths be taken into account? Is this generally based on estimation or engineering judgment?
Post
The main point is that you need thermal symmetry between the two pads of a small package. You want the solder paste to melt at the same time between the two pads.
Molten solder has significantly higher surface tension than solder paste. When the solder melts, the surface tension will try to "lever up" the component from that end. If the other end is also in molten solder, then the lever-up torque of both ends cancel, and the surface tension at both ends keeps the component on the pads.
When one end is molten but the other not, then the component can get flipped up to stand on the molten end, which is called "tombstoning". As you say, this can start to happen with 0603 packages, and is definitely an issue with 0402.
The issue with planes is that they have more thermal mass than the fiberglass board, and therefore heat up more slowly. The thermal reliefs you show are meant to thermally decouple the pad from the plane somewhat. The more thermally isolated the two pads are, the more they are going to heat up on their own, and therefore closer to the same time.
Since planes heat up more slowly, there is more opportunity for a time difference to reach the solder melting point when there is a little imbalance. For this reason, it still makes sense to include some thermal relief, even when both pads are connected to large planes.
The pads in your top picture look good. R10 in the second picture might be a problem. You have decoupled the top pad from the plane, but there is still a more significant thermal connection to a larger area of copper than the bottom pad. Will that matter? Probably not in this case, but you'll have to see how 100 boards come out to know for sure. It seems you have lots of room. You could use a 0603 there instead.
If you are using lots of small components and are therefore worried about tombstoning, you should have a talk with whoever is doing the assembly. They should be doing this anyway, but make sure they are using the right heating profile in their reflow oven. They should get the temperature to a plateau just below the solder melting point, before advancing to the melting phase. Using solder with a low melting point makes this easier without over-heating the components. Make sure they are using a temperature profile optimized for your board and their solder paste, not just something generic.
I don't really agree with the twisting shown in the bottom diagram. Yes, the melting will be a little off-center initially, but with a proper solder mask, there shouldn't be any twisting force once the solder has completely melted on both pads. It's interesting that they don't show the solder mask at all, which is quite important when considering twisting. If the solder mask openings are only over the metal pads (or close to them), then the component will actually align itself properly when all the solder is molten, even if initially placed a little off.
The only rule of yours that makes no sense to me is that thru-hole pads should always have thermal reliefs when connect to a large area. I don't see what issue this is intended to address. Also, anything with thru hole pads is going to be significantly larger than even 0603. Surface tension of molten solder will be small compared to the weight and other forces on the component.
3 comment threads
0 comment threads