Question about connection between via and filled zone

Hello everyone,

I’m designing a 4 layer PCB and I have a problem when I use filled zone function on the middle layer. This filled zone will work as ground plane of PCB.

So, my question is that how do I set up the filled zone to achieve a connection between the via and the filled zone similar to the figure below?

My design is shown in the figure below and doesn’t have the hollow area like the one above.

One more question, why use the connection method in Figure 1, will it reduce noise or reduce heat generation?

Best regards,

In the zone properties / pad connection you can select thermal reliefs (yellow picture) or solid (green picture). If I understand you right, that is.

Solid connections have a lower resistance and inductance. Usually this is only an issue for high current or high frequency applications.

For through-hole pads: they are harder to solder without thermal reliefs as the solid connection to the plane dissipates a LOT of heat.

Thanks for your reply.

I have selected thermal reliefs, but the filled zone remained the same structure.
It works with pad, but doesn’t seem to work with via.

Do I need to adjust via properties or do some other operation?

Honestly, I don’t know. To me thermal reliefs for vias are pointless as they are never soldered. @paulvdh?

Ok, thank you very much.

Here you do not want thermal reliefs.
Vias in thermal pads steal solder, so unless you are planning on the expensive filling and capping options, I recommend using a small drill size eg 0.3mm. Most low cost PCB fabs can do this.

If you don’t know about this subject, I don’t know if the question was answered clearly enough.

Vias are part of tracks/zones, they just connect copper between layers. Through hole pads are used for THT component leads, mounting holes etc. Thermal reliefs, those copper spokes with copperless space between them, are used only for pads, and even then for one special purpose only. When you try to solder a THT component lead in a through hole manually, you have to get as much heat from the soldering iron to the solder, pad, and component lead, but not elsewhere. All copper conducts heat, and a solid copper connection leads the heat immediately away and is wasted, making soldering difficult. When part of the copper around the pad is taken away, less heat goes away and soldering is easier. All other effects of the thermal reliefs are unwanted, unnecessary or negative. Therefore you should use thermal reliefs only for manual soldering. Sometimes for SMD component pads, too, if you solder them manually.

In KiCad vias don’t even have properties for relief connection, so when you want thermal reliefs, you have to use footprints/pads. When you use vias to connect a track or a zone to a plane (zone), you certainly don’t want to use thermal reliefs because everything they do is make current flowing harder, while the purpose of a plane is to make it as easy as possible.

1 Like

→ make heat flowing harder.

Well, yes, it’s everything which it’s supposed to do. But when there’s no need for thermal function, everything what it may do is make current flowing harder. Whether it has any noticeable effect is another thing, but they still break the continuous plane.

So it wasn’t a slip of the tongue.
I got it from dictionary - not sure if can be used to something written and not spoken.

OK, thank you for your patient explanation.
So the thermal relief seems to only work with manual soldering.

Sorry, I have another question, if a QFN package component requires thermal vias to be added to the pads in the center of the footprint like figure below. So in Kicad, should I add vias or through hole pads like in figure 2?

Thanks for your reply.
Is it ok to use 0.5mm as via diameter and 0.2mm as hole diameter?

Depends on what you are ready to pay for a board. For cheap boards it is 0.6/0.3 for 2 layer and 0.45/0.2 for 4 layer (JLCPCB)

Afaik there are QFN packages with thermal vias in the footprint library.

1 Like

It minimum drill size depends on your supplier and how much you are willing to pay for a board. The cheap ones stop at 0.3mm

If you want to have the thermals always in the same place and size, you can put them in the footprint as through-hole pads with the same pad number as the thermal pad. I usually don’t do this though – I place them as vias in the board editor. This lets me tweak the position of the thermal vias to match the situation of the specific board (for example, to clear critical placements on other layers)

This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.