How do they say, an image is worth more than 1000 words…
To bad the new pad shape of rounded corners (fillet) doesn’t allow chamfered edges…
Or alternatively an octagon as basic shape with round corners 
3 Likes
When there are vias within the thermal pad i’ve found that a large amount of the solder paste goes through to the other side of the PCB which can cause problems - to stop this putting solder resist over the vias works well but printing over the solder mask can lead to voiding.
One solution when the vias have been masked is for the stencil to be designed to avoid the mask areas as shown below
See article - http://www.surfacemountprocess.com/a-guide-to-effective-stencil-design.html
1 Like
I’m new here (just download KiCAD tonight), and I came across this post trying to learn the ropes. I had been using EAGLE for work, but I’m not a fan of what Autodesk did with it. I can’t offer much in the way of how to do it with KiCAD, but I thought I’d offer my two cents from an assembly standpoint. Briefly, I’ve been designing PCBs professionally for four years, and I’ve been through the issue of thermal vias in pads many times in my work.
There are a lot of answers to this question, but one thing to consider is how hard you plan to drive the chip. If you aren’t going to be pushing the chip to its limits then you may not even need thermal vias. Check your datasheet for thermal information before taking this suggestion. I always prefer to design them in… just in case. Another thing to consider, as others have mentioned, is how thick are your various layers of solder paste, solder mask, etc. One thing I did not see is to make sure that your board house can actually build it. There are minimums that they can have for spacing between copper pads, pad edge to mask edge, mask thickness, trace thickness, etc. I’ll try to find some good references with more details on this, but that’s how board houses charge. They’re not willing to give it up lightly. Generally, the more lax your requirements are the cheaper the board.
Speaking specifically about vias, as you showed in mid Feb there are several options such as tenting, copper plating, etc. My experience is that tenting and plugging do not add anything to board cost. When you start adding more conductive material, it can be an enormous charge. The most cost-effective way I have found thus far is as follows:
Use a solid thermal pad on the copper layer. Create a cross-hatched pattern of solder mask OVER the thermal pad. Use two strips of solder mask in both directions which divides the pad into 9 equal parts. Place four thermal vias in the four intersections you created with the solder mask. As far as the paste layer, I’ve seen a lot of suggestions, but the type of finish you have can have an impact on this. I’ll explain that in a second. I would suggest making the paste layer a few mils in both dimensions smaller than the remaining exposed copper. I’ve seen anywhere from 40 - 70% as being acceptable. When you have your board built, ask for tented or plugged vias.
The finish of your PCB may also have an impact on the solder coverage percentage. A PCB finished with ENIG (immersion gold on nickel adhesion layer) will have a smoother surface, and it is preferred by assembly CMs because it improves solderability and shelf life. It is also more costly. If you are buying this from your own pocket you might opt for a HASL (hot air surface level) finish, but this will result in a much rougher surface. For a few boards it wouldn’t be as much of an issue, but if you plan on running 100s go for gold. My gut feel is that with a HASL finish you would want closer to a 70% solder coverage, or at least a thicker solder paste layer.
I apologize for the novel and the lack of pictures. Like I said, I’m new to KiCAD. I know a picture is worth 1000 words, so I will try to get a footprint put together this weekend. I hope this helps (even if a little late).
1 Like