Via near micro Pad cause problem or not

Hi all
I have a question regarding via near pads of mcu?
could it cause problems?
Thanks

Yes, it could, but only under certain circumstances. What’s your case?

1 Like

Thanks I have a stm8 micro the pakage lqfp the distance between pads are 0.2 I want to set via so I can increase the size of track on the bottom of the board

A screenshot might help.
And we might also need information about how you intent to solder your pcb.
We would need to know if the vias can be tented on the side where your pad is. (if they can be covered with soldermask.)
Maybe also what the drill size will be.


One way a via can make problems is when you use reflow soldering. If there is an open via near or even inside the pad it might wick away parts of the solder paste. This could result in unconnected leads.

The best solution is to tend or even fill the via. Another option is to decrease the drill size. (Might not always work as the minimum drill size of the board house might still be too large. Requires testing.)
If all of this is not possible you will need to ensure the via is far enough away such that solder mask can be between the via and the pad. (It might be enough if the drill is guaranteed to be outside of the paste covered area. Again this would need testing to ensure you get the expected yield.)


Another possible problem is that too many vias placed too near to each other could split up a copper plane. This might result in EMC problems.


If you have untented vias you could run into problems regarding minimum soldermask width. So it is (in theory) possible to have no soldermask between neighboring pads. (Can only be a problem if your track clearance is smaller then the sum of solder mask clearance plus soldermask minimum width.)


If you handsolder it might increase the probability of you making solder bridges. (Again only a problem if your via is not tented.) Especially if you have the via under the part body. (It is then hard to see if you indeed create a solder bridge.)

4 Likes

Thanks alot Rene for your complete answer

One more comes to mind. If you have a component with a metal part under it touching the board - i.e. an exposed pad - and you don’t have a corresponding pad in the footprint (because it’s not needed in your application) or it’s smaller than the component’s pad, and try to save space by putting tracks and vias under the component, a via may be incompletely covered by the solder mask and create a shortcut when it touches the thermal pad. I have heard this has happened. If you look at some boards with vias you may notice that the solder mask is thinner on top of a via, especially in the edge of the hole, than on top of a track.

2 Likes

This topic was automatically closed 30 days after the last reply. New replies are no longer allowed.