My main question, should I use thermal vias, and solder through the back of the board to solder the thermal pad to the board?
The data sheet for this TI, TPA3110D2, calls for solid vias. I would like to explain what I think I know, and it would be appreciated if someone could steer my thoughts in the right direction.
Solid via; would need solder paste and heat gun to solder onto the board, but provide great thermal conductivity.
Thermal vias; not sure how to solder the thermal pad to the board, if these vias should remain open to let heat escape.
Thermal pad is just the pad thatās on the back of the IC. but that should be soldered to the via (but not a thermal via?)
Filled areas in zones is checked. But if I uncheck āsolder paste layersā I can see my vias. So now Iām searching for solder paste layers and learn about themā¦
As far as I am aware KiCad does not even cater for thermal relief vias.
In your case everything is as it should be.
If there are vias in filled zones under a chip they would be covered by the paste layer in the 3D-viewer.
Vias in general have solid connections since they are not meant to be soldered on, except when present as part of filled zones under chips. Purpose here is to have a solid connection acting as a heatsink to the chip.
It is also a good idea to keep the paste patch under the chip rather smaller. Reason here is that too much paste makes the chip simply float, or even drift off. If the chip manages to just float high enough there will be hardly any connections to the pins, and the pain of fixing that mess sets in.
Part of the confusion is terminology. You need thermal vias to get the heat away from the chip. The point emphasized by the data sheet you quote is that you shouldnāt use thermal relief in those vias. (To add to more confusing terminology, some people call them via thermals !). These are the webbings that attach a via to surrounding copper. Solid via means a solid connection, no webbings. (It is not about filling the via hole with solder).
And as Jos mentioned, when KiCad makes vias within a copper zone, it is solid by default.
You need those webbings ā call them thermal relief, or via thermals, as you wish ā when attaching through hole parts to largish copper zones or fat tracks. Makes your life less interesting while soldering and āeven moreā less interesting while desoldering. Attaching a picture so you get the idea.
Depends somewhat how much and exactly where the paste needs to be without having the chip take off.
I can guarantee you that if you would cover the whole thermal pad with paste you will run into fab-issues. Especially with small VQFNās and such. With too much paste the surface tension (during the reflow process, far worse with hand technics) may not be enough to actually pull down the chip.
Most application notes i have read regarding this suggest somewhere between 50 to 80% area coverage depending on stencil thickness, solder loss through vias, ā¦
It is also a good idea to split up the paste pad for such a large pad as it better allows gases to escape and it also reduces the chances of paste being scoped out by the squeegee. (I personally aim for 1 to 1.2mm side length for these smaller pads.) All of this is explained in great detail in the tutorial linked above.
Exactly. I only scratched the surface. There is more, we have influences like room temperature, air pressure, moisture in the air and moisture on the board, dust, shape/tension within the board, surface, paste, the process how the paste gets onto the board. Did I miss something?
As for belly-pads, I always break them down in small patches. For SMD pads in general I take off at least 10% paste. 61.8% seems to be the best ratio.
I think anything what was said was about how it should be done for normal automatic production.
The vias has to be no bigger then 0.3mm to not stole the paste during reflow soldering. The paste should be not too much to not make shorts to other pads.
I know (I have never done it myself) that amateurs who hand-solder such footprints do things differently. In such footprint there would be probably two vias in thermal pad big enough to solder to the thermal pad from backside. The thicker the PCB the bigger via is probably needed to see that you soldered successfully to thermal pad. I think such vias can have diameter of even 5mm if thermal pad is big enough.
This will give the IC the enough good thermal connection to GND copper at backside. It could be used in production I think, but it would need these vias to be hand soldered so would be more expensive.
I removed the vias and added pads of 0.5mm in the foot print. Iām not sure if Iām at 60% pad size for the paste area, but I did make it smaller. I submitted the boards yesterday for manufacturing.
Thank you everyone for the input! Iām not 100% with this area yet, but I have a better understanding.
Last time I remember that I have to use wizard to create a new footprint, and to copy and paste or text editor to move it into the existing footprint. Is this now get easier?
The thing i linked above is a standalone python script. It outputs a footprint as defined in its input files. (see documentation pull request also linked above for access to a preliminary documentation.)
