Continue to Site

Welcome to EDAboard.com

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.

Can I place vias through SMT pads?

Status
Not open for further replies.

Jos Brink

Member level 3
Member level 3
Joined
Jan 28, 2004
Messages
64
Helped
9
Reputation
18
Reaction score
2
Trophy points
1,288
Activity points
577
Can someone tell me if it is ok to place via's on SMT pads.. ?

Thanx

Jos Brink
 

through pad smt

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.
 
can have via under smd pad?

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.
 
smt pads

thnx.. i changed my pcb..
a PCB manufacter told me it was ok to do it.. but i had my toughts,,

lesson 1: trust no salesmen.
 
force complete tenting via

What are plugged vias?

best regards
 
through hole via blind via rf

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.
 
via size smd

In Altium there is an option called force complete tenting. That will cover the top or bottom of the via with copper, and you won't see hole.
 
via in pad

HI,

As vvv says in his reply,you can have via on the smd pad,but then use filler to fill it.

Since you have filler in the via,it will protect while paste melts and wick up into the via.

You can collect the information of the filler from ur fabricator.

Regards

Ramesh
 

bga blind via reflow void

You can place micro vias on SMT pads.

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.

I hope this is helpful to you
 

altium designer micro vias

This is not recommended. VVV is 100% correct, will give you lots lost of problems !.
 

many vias in smd pcb

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.
 

Status
Not open for further replies.

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Back
Top