Thermal Pad/Reliefs design?

[mImoto]

Hello,

I would like to know how to design (dimensions, ¿square or circular?, etc) the thermal relief/pads of the through-hole components and vias. I would thank you a lot any paper, link, tutorial, etc.

Thanks a lot and best regards,

mimoto

 

[House_Cat]

The reference is IPC-2222, page 16-17.

Take a look at: **broken link removed**

 

[mImoto]

Hello,

Could you explain a bit more please how to design a thermal pad from the *IPC-2222*. I have look at it but I don't know how to obtain from it the internal and external diameter of my thermal pads and also the slit width.

Thanks a lot,

mimoto

 

[House_Cat]

There isn't much to add to the IPC explanation.

Your question makes it sound like you don't have much experience with printed circuit boards.

A thermal relief is used to allow easy soldering to through-hole components. A direct connection to a plane sinks much of the heat applied to the joint, and makes it difficult to solder without overheating the component and board.

Every component pad has some minimum copper annulus required to ensure both proper plate-thru of the hole, and to ensure mechanical strength of the solder joint. Those numbers are also called out in IPC publications. Your EDA software should have some library components where this part of the work has been done for you.

Once you have the annulus size, you need only concern yourself with the maximum current, and the reactance your application can tolerate for signal integrity. You can then chose the number of "webs", or radial traces you will use to connect to the plane.

From the above starting points, you just plug the IPC equations in the reference I gave you. The final step would be to simulate the pad in the appropriate signal integrity software to make sure it gives you the desired results.

If your application isn't signal critical, then just use four radials of about 10mils width, and annulus of at least 10mils around the hole. That will get you by for soldering purposes, but it probably won't do too well for fast or high current signals.

The bottom line is - this is science, you need the background to understand what you are trying to accomplish. There isn't any cookbook that will do the job for you.

 

[amjad]

For example in the pads software these dimencions and shapes can be given in the padstack definitions.Similarly in other softwares also there are padstacks in which yoc deifine them

 

[ahsoka]

Hi house_cat,
its a good point you made.
but i have a doubt....??

why do we add thermal relief pads for THD?? why not for SMT???

thanks in advance

 

[karesz]

Hi,
If you are a good layouter, your SMD pads has some similar constructs too...
Of course must you have around an SMD pad a thermal relief similar solution; otherwise you (or maschinell) will ther not can older:-(
K.

 

[pcb-lab]

Maybe it will be useful to try the LPCalculator: http://www.pcbmatrix.com/Products/LPSoftware/LPCalculator/

 

[FvM]

why do we add thermal relief pads for THD?? why not for SMT???

You apparently mean pads surrounded by a copper pour? Most CAD tools are providng thermal isolation for SMD pads as
they do for throughole. But you may want to disable it at least for some SMD pads. In contrast to wave soldering of
throughole pins, reflow soldering of SMD pads works without thermal isolation as well, because the board is heated as a whole.
Prototyping and repair solder possibly needs preheating of the board.

Some reasons to omit thermal relief for SMD pads:
- lower thermal resistance for power devices
- lower inductance for bypass caps
- better connection of high current devices

 

[karesz]

Hi,
What about tomb stones & homogenous soldering quality pls?
K.

 

[FvM]

I didn't yet observe differences in soldering quality between "isolated" and SMD pads in a copper poor or hear complains from
assembly service providers, although they complain about a lot, founded and unfounded things as well. I don't even know, if
there's a considerably difference in solder melting speed. The differences between parts of different thermal capacity are surely
more important in practice. Tombstoning is rather a problem of unsuitable pad respectively solder mask shapes in my opinion.

But anyway, the reasons for non-isolated pads are counting on their own. I didn't opt for flooding all SMD pad's thermal reliefs,
you have to find your own tradeoff.

 

[kannansha]

Hi all

Do any one know how to provide thermal relief to VIA's in Protel 99SE. i can able to achieve that for SMD and through Hole PADs but not for VIA's alone.
if anybody have solution for this please help me..

Thanks in advance
sha

 

[khanna_gunjan]

Hello Kannansha,

I am not sure, but probably you need to check your design rules for polygen connect. probably it is defined as direct connect for vias.

 

[kannansha]

Hi Khanna

Actually i checked at Design Rules and i fixed it as Relief connect only not as Direct connect, but still that problem occurs, the Reliefs comes at all other Through Hole pads but not only for VIA's. but i found some other way to solve ths issue..:razz:
Thanks for reply

Sha