Thermal relief vias

[occam25]

Hi,
I am using the TPS63020 buck-boost converter in a design and the datasheet recommends to place several 0.2mm vias in the exposed thermal pad for thermal relief. My question is about the annular ring of those vias. Do thermal relief vias need annular ring? I guess not because they are in a pad, so there is copper already, but what about the via's internal copper? will it still be there if I remove the annular ring?
When I say "remove annular ring" I just mean to define the via's diameter the same size of the hole. Is this the right way yo do it?

Thanks!
Javi

[robertferanec]

You can simply place into exposed pad standard VIA, you do not need to remove VIA pad (ring), unless you have very specific reason to do so. I always use standard VIAs in exposed pad, no problems.

PS: Some people will recommend you to fill the VIAs under exposed PAD to prevent solder to flow through the VIA, but this may make your PCB more expensive, so you may only need it in special cases (I do not fill 0.2mm hole VIAs under exposed PAD and we have not had any problems with that).

[occam25]

Thanks Robert!
Is there any reason that makes the annular ring removing not a good idea? I can use a standard VIA, but removing the annular ring allows me to place them closer and to increase its number. I am considering that because in the datasheet's suggested land pattern (see attachment) they place 15 VIAS!! although it is probably not needed to place that many.

I guess that the best way to evacuate the heat is to place through hole VIAS, but this is a high density design and I can not avoid to have components in the oposite side of the board, would it be enough to use vias from the top to a internal ground plane?

Thanks for your support!
Javi

[robertferanec]

Is there any reason that makes the annular ring removing not a good idea? I can use a standard VIA, but removing the annular ring allows me to place them closer and to increase its number. I am considering that because in the datasheet's suggested land pattern (see attachment) they place 15 VIAS!! although it is probably not needed to place that many.

It is the same net, so you should be able to place standard 0.45mm (VIA pad) / 0.2mm (VIA hole) VIAs into 0.5mm pitch without any problems and violations.

If you make the ring too thin or if you remove it, PCB manufacturer may start asking questions about what it is or they can tell you, that they can not manufacture a via with so thin ring (because of drilling position tolerance). Unnecessary questions from PCB manufacturer is the only reason why I would not remove the ring completely.

I guess that the best way to evacuate the heat is to place through hole VIAS, but this is a high density design and I can not avoid to have components in the oposite side of the board, would it be enough to use vias from the top to a internal ground plane?

I do no know if that would be enough to take away all the heat. Also, you would need to use blind VIAs and go into your GND plane - that may make your PCB more expensive and I am not sure how big the hole inside blind VIAs would need to be. You would need to discuss this with your PCB manufacturer.