Display Your Know How: Thermal Relief

Hi this is fairly easy to do within Orcad / Allegro. If using Allegro 17.2 and above you can change the pin properties so that the thermal relief is not needed, To do this select pins in the find filter then right click on the pin and choose property edit. Next assign the property of Dyn_Thermal_Con_Type and choose "none" for the layer you wish to remove the thermal from. Typically for thermal reliefs as in the picture there is a net associated with the pin so the net will still need to be connected on another layer.

This only works for dynamic planes. If using Static planes there wont be dynamic thermals connecting to the pin.

Best regards.

Thanks for pointing this out excellon1 ! Yes it is easy to do manipulate the thermal relief property of pins in OrCAD and Allegro. But the question we would like to focus on is: should we?

For electrical and thermal performance, the thermal type "Full_contact" is superior. This begs the question, why do we use thermal reliefs at all? Why not simply use full contact for shapes at all our pins?

And what PCB design choices can we make to achieve this (if required) without compromising the automated assembly process; any suggestions?

Thanks for your input excellon1. These insights are greatly appreciated!

In the image above used for this question, we show two different pin types: through-hole and surface. Focusing on the surface pins: do you see any other layout solution that would enable us to use full contact on the surface pins while encouraging good soldering? ( hint: imbalance)

One key point we would like to highlight is that thermal reliefs on surface pins vs those on through-holes combat slightly different problems. The reason for their use is not exactly the same for each technology. Kudos goes to anyone that can think of what that difference is...   

Hi PCBTech.

Good questions. Looking at that particular design I would go with direct for both the smd and surface pins. From the soldering
perspective you are looking at a really small copper surface area so soldering wont be any problem for even a budget rated IR oven.

Basically because the copper surface area is tiny IR Ramp up will be fine.

Best regards.

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?

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.

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.