Display Your Know How: Thermal Relief

Hi again PCBTech.

One thought I forgot to include is a question.  On this small part of the design do thermals make any sense at all ?. I don't see that they do. As above the thing here is the really small copper area used. Direct connect is a far better option IMHO. Personally I typically favor
max copper in any design.

One other thought on this. Within Allegro the default for thermal relief is Orthogonal. It could very well be that the designer may not even been aware of the direct connect option. It looks like someone just poured a dynamic plane and the thermals appeared to tie the nets in to the small plane. :)  Kind of like pressing the go button, hey it looks good to me lol.

Looking forward to your feedback.

Best regards.

Hi excellon1, we are loving this discussion. Thanks for all your inputs! You make a good point about the area of the copper. Yes the through-hole pin may not need thermal reliefs for this connection to the copper plane if this is the only copper layer connected. As in the case of through-holes, thermal reliefs are used to prevent heating escaping from the hole during soldering. This enables the local region to heat sufficiently such that an inter-metallic bond can be established between the solder and the metal surface of the inner hole. 

It should be noted that in this case, the heat source is the solder! However, for surface mount production, the solder is not fluid and so the heat energy is provided from the atmosphere, not the solder. Therefore surface mount pads use thermal reliefs for a different reason. 

Back to the topic of through-hole pins: In the first image, there are still some things that we cannot know. For example - how thick is this copper? Secondly, is this copper plane on the topside or the soldering side?

(We shall assume this must be an outer layer due to the surface component nearby. However, embedded layer pads area possible using Allegro PCB Editor - but let's assume not in this case....)

Do you have any thoughts if these factors should affect your decision about removing thermal reliefs?

Also, do you know any other pin technology which could be used to avoid this entire dilemma?

Gold star answer - thank you FalcomPeter !!

Agreed, changing the narrow trace on the right side pin of the surface mount component will help to balance the thermal properties of this part which will help production. You have rightly pointed out that the issue of tombstoning is of concern for discrete component types. This phenomenon describes components that lift on one side due to a timing imbalance of soldering between different pins. The finished PCB may look something like a graveyard if lots of "tombstones" are sticking up in the air indicating a dead circuit due to these broken connections.

It is caused when one surface pad heats up much faster than the other. The melted solder pulls on one side of the component due to surface tension and buoyancy. Without a counteractive pull from the other unmelted side, lightweight components will rise into the air. Videos of this phenomenon are available to view on public channels such as youtube. 

Question though: which side heats up quicker - the side with wider copper or the side with less copper? Remember the heat energy comes from the atmosphere.

Do you have any thoughts on the through-hole discussion? Any insights would be very welcome. One point we would like to mention is the assembly technique known as "intrusive reflow", Some manufacturing engineers also name it "pin in paste". 

Example of thermal balancing of smd pins with no thermal reliefs (full contact with copper planes)

HI JCTEYSSIER0, thank you also for your inputs! It seems that these reasons also relate to manufacturing performance more than electrical performance. Would you agree?

An interesting point that you have brought to mind, is if any designers ever consider blocking heat from travelling into a pcb due to electrically generated thermal output of components. It is conceivable that heat could be channelled away from the pcb by way of direct contact with the surface of a component with a heat sink for example. In that scenario, perhaps we can imagine the requirement to reduce thermal transfer through the pcb for heat dissipation.