There’s a lot going on in this thread and many different connector models. Make sure you know what you are really using. Even that datasheet describes more than one model.
This picture below that text shows a completely different part.
These two through holes must be there according to your datasheet. But the footprint is for the SMD version of the part. Make sure you have the right one.
But I don’t think that’s what Piotr meant. I think he meant having extra vias in the SMD pads or touching them so that the same solder tin slump which fastens the part pad goes through the board, too.
In te image below there’s pre-applied insulation on top of the part. The bottom is metal, and in my experience usually is in these kind of connectors. BTW, this isn’t a standard USB connector but a 10-pin connector which probably is compatible with a normal USB plug.
Most often surface mounted USB connectors are OK, but through hole versions are stronger. We have had problems with some products - SMD connectors were broken off when a user had to use some force in certain situations. Through hole connectors stay there much better. We try to avoid SMD connectors if possible.
Referring to you datasheet, we would use the SM1 type, not SM type.
No. Your solution in my opinion gives nothing.
Read once more:
So in total 8 vias.
My vias are 50/28 mils and connected to pad by 50 mils wide track.
They are placed such way that hole is just touching the GND pad.
I can’t give the picture as I’m at home. Even at work it is a little time consuming as I work at PC not connected to net.
You can use 4 vias to each pad.
I have read that via in pad have to have hole smaller than 0.3mm to not ‘steal’ the tin in reflow soldering. In this case I added bigger once so not placed them at pad.
I covered my vias with soldermask. I just believe that metalization going to next size helps to not rip pads off board (that this metal is stronger than glue keeping pad at PCB.
I have never done any experiments in that subject. I just now that a small SMD pad is very easy to rip specially if during hand soldering you heat it too much.
There are tens of different (maybe even 100+) footprints for USB connectors, so be very carefull with just grabbing a footprint from KiCad’s libaries.
For pure SMD connectors it is wise to put a few via’s directly through the mechanical pads to strengthen them. (Not connected via a trace!)
It is also common that these connectors are mixed THT & SMD.
SMD for the electrical connections.
THT for (some of) the mechanical pads.
But also:
Via’s directly through pads can (and will) wick solder paste, which can (and will) also weaken the connection. This is sometimes solved by making the soldermask bigger then the pad. During soldering the solder will get wicked onto the pad. To do this right will need some tinkering, or a lot of experience.
