Welcome to our site! EDAboard.com is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.
This is not recommended.
When the paste melts, it will wick up into the via, resulting in a poor solder joint.
In fact, vias should not be placed even close to the pads. A minimum of 0.005~0.008" is recommended, for similar reasons, especially if the vias are not covered with solder mask.
If you need to have vias at the pad, it is recommended that they be plugged vias.
Microvias are OK, but as VVV say's they should be plugged. If not, air that gets trapped in them will form bubbles and "explode" during reflow soldering.
Plugged microvias are filled with copper. I have seen buried vias also filled, but with other materials. This in order not to have trapped air inside them.
A common practice in RF designs is to pour copper around all SMD's on the TOP/BOT layer and then by the use of micro vias quickly go to the inner layers in order to reduce radiated interference.
Also you can place normal vias, but you need to plug these holes and plate the surface, so that the vias will not cause any problem during assembly and on the field.
For plugging, the PCB manufacturer can plug with epoxy material. This will be done after drilling vias and plating the walls of the vias. After plugging they have to do the plating again.
Like many things in the world of electronics, facts and opinions change as time goes by. Via-in-pad can be used if you know what you are doing. As long as the hole is not large compared with the size of the annulus, solder thieving and bubble formation will not be a problem. Large can be defined as about 25% of the exposed copper area.
As an example of the change in thinking regarding this subject, here is a quote regarding via-in-pad for BGA mounting taken from pages 28 and 29 of the latest version of IPC 7351A - Generic Requirements for Surface Mount Design and Land Pattern Standards (dated February 2007).
Via-in-pad (through-hole via, capped on bottom of the board) can cause voids in a BGA solder joint, which may impact reliability. Current data indicate that, for the standard 25 - 35 mm package with 0.75 mm balls, there is no reliability risk from voids. Accelerated aging tests have been performed and the failure rate was statistically equivalent to standard dog bone designs. It appears that void consistency is more important than void size with respect to solder joint reliability. Most experts agree that these void conditions, created due to entrapped air, are acceptable and have no impact on the reliability of the joint. There is no doubt that the conditions depend not only on the process, but the size of the land and the diameter of the hole. In addition, there is a difference as to whether the hole is a through-hole, blind via, or microvia.
This site uses cookies to help personalise content, tailor your experience and to keep you logged in if you register.
By continuing to use this site, you are consenting to our use of cookies.
