Thermal Relief – Yes or No?

[Eyal78]

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?

Image 1:

Image 2:

Image 3:

Thanks in advanced for any answer!
Eyal

 

[wwfeldman]

no idea - but if you look, you can find information

try this

Tombstoning - Eurocircuits

Tombstoning is also known as the Manhatten Effect is an issue that can happen to a SM component during the reflow soldering process.

www.eurocircuits.com

 

[ahsrabrifat]

With reference to Image 1: C14, C15, C16, C17, thermal relief is recommended here. Direct polygon connections can cause asymmetric heat dissipation.
In image 2, R10, Thermal relief is recommended for the connected pad. In case of C12, R11, thermal relief is not necessary because neither Pad is connected to a Polygon.

 

[D.A.(Tony)Stewart]

The biggest failure in mfg are solder defects, insufficient, excess, bridge, intermittent, and tombstone, but design margins help improve yield.

When you chose your design for high density pads like this, consider the cost of rework. Consider changing your library pad choices. See the gap and pad around outside!!

Consider pads for medium or robust pads if you have the space. ref https://www.protoexpress.com/blog/pcb-manufacturing-defects-caused-land-patterns/

Your best bet for ensuring reliability is to use footprints designed to the IPC-SM-782 Surface Mount Design and Land Pattern Standard

 

[KlausST]

Hi,

Yes, IPC is a good reference.

***
From my own experience: In my early SMD days I thought the bigger the pad the better.
And I agree for hand soldering each pad .. it´s more easy.

But for reflow soldering .. there definitely is a "too big" for a pad. For low soldering errors .. bigger is not better.
A bigger pad may be mechanically more robust .. but still there is a higher risk for thombstoning, moving, no connection...

Klaus

 

[marce]

Nope, like many SMD SMPS, you don't need thermal relief. I never use it on SMD components and have never had any issues with assembly, never had skewing or tombstoning on small SMD chip components. With the correct soldering profile, you should NEVER get a temperature gradient across a small chip device, both pads should wet and reflow at the same time.
This has applied to mass manufacture and high reliability (Class 3) designs, manufactured in their millions or expensive 1 offs...
On image 2 I would move the device away from the polygon and use a track, if you are worried.
During reflow soldering the whole design is brought up to the same temperature at the same time, to avoid thermal shock and avoid differential temperature across components (differential temperature across a component is a sure way to get failure). In the early days of reflow soldering (1990's), infra red ovens and lack of pre heating zones could lead to quite harsh soldering conditions and steep temperature gradients across small sections of boards. In those days I preferred and used vapour phase soldering, as it was a better system. Todays reflow machines are far more intelligent, with better profiling and control.