Confused by black layer around GND pad

For me the copper heat sinks belongs to the footprint and should be included there.

In your footprint, you can place 2 Pads on top of each other, both with the same pin number, one for the heatsink which is larger than the other, on this one you should disable F.Mask and F.Paste. Then you also don’t have this problem.

Not the best idea as that way you fix the heat sink shape, while at each PCB you can have different shaped area to use. Copper pour are more flexible.

@johannespfister I agree with you that I could have put it in the footprint. I saw tradeoffs to both approaches and decided for now just to do the manual copper pour.

Your second paragraph really confuses me. If I were to make 2 pads, one electrical and one heat spreading, and then disable the solder mask on the heat spreading pad, there will obviously be no opening in the stencil for solder paste on the heat spreading pad. This will lead to no solder on the heat spreading pad.

Without solder, there is no bonded metal-to-metal connection between the hot region on the IC and the heat spreading pad. What will conduct the heat from the IC to the heat spreading pad? Thermal grease is not an option here because it will not survive reflow.

I’m either not understanding your method here, or I am understanding it but am confused about how it will promote heat spreading given the lack of metal-to-metal contact.

The 2 Pads overlap. One of them has the F.Mask and F.Paste active, in this region the IC is connected to the copper. The other pad which overlaps is bigger. It doesn’t change the F.Mask nor F.Paste, so there is still a connection from the IC to the Pads.

Thanks @johannespfister . I thought you were describing two pads that were not connected to each other. Makes sense now.

@paulvdh I am still slightly confused about thermal reliefs and whether I want them or not. Maybe you or someone else can help me understand.

I do want to use the pad as a heat sink to spread the IC’s heat to the other copper layers of the board. So, based on your message, it sounds like I want to disable thermal reliefs on this pad.

However, won’t this make it more difficult to reflow solder the pad? The solder’s only boundary will be the solder mask surrounding the pad, so it will be a solder-mask defined pad. When the solder melts, will it flow out of the pad and onto the surrounding mask? Or will the mask prevent it from flowing outside of the pad?

In short, I need both heat sinking from the pad to other layers, and easily solderability. What should I do?

Then it is simple. You can not use thermal reliefs if you want to use the copper zone around the pad as a heat sink.

No. With reflow, the whole PCB is heated at the same time, and thermal reliefs have no effect.

Thermal reliefs are only important for manual soldering. If you are heating a pad with a soldering iron, then a pad connected “strongly” to a big piece of copper is difficult to heat enough.

So, jjust to be clear: Thermal reliefs are only useful for manual soldering.

1 Like

Excellent answer. Thank you very much.

1 Like

I’m pretty sure, paulvdh meant “thermal relief” where he wrote “thermal via”…

This is not strictly true.
Through-hole assembly by automated wave soldering can also benefit from thermal reliefs. As always, consult with your assembler before doing a layout to determine their best practices.

1 Like

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