What do you think of "It is not recommended to add vias on SMD pads"

qwqwqw2088

What do you think of "It is not recommended to add vias on SMD pads" [Copy link]

 

Recently, because I have made a lot of boards at a certain board manufacturer, when I asked them for technical support, they had a suggestion, which is "It is not recommended to add vias on the surface mount pads"

In addition, they also found some illustrations and precautions and shared them for everyone to discuss.

Manufacturer's suggestion: It is not recommended to add vias on the SMD pads.

Here are the reasons:

Before machine mounting, solder paste needs to be printed on the pad, and the solder paste will melt into liquid during reflow soldering;

If there is a via on the patch pad, the liquid solder paste will flow out of the hole, resulting in an open circuit in the pad's solder joint.

okhxyyo

This is true. If you want to drill a via on a SMD pad, why not just make it a via pad?

bigbat

This is a hard rule for me. There can be no vias (>15mil) near the pads, and the copper connection must use flower pads. Because I have suffered losses, of course, except for the particularly large pads and plug-in installations. Some need heat dissipation holes. The high temperature of lead-free soldering can easily cause cold soldering, and it is particularly difficult to detect.

bigbat

okhxyyo posted on 2022-10-8 15:53 This is true. If you want to make a via on the SMD pad, why not just make it a via pad

It is recommended that EEWORLD create a PCB standard process, such as the pin position of the component, the symbol positioning of the diode, the board frame standard, via, line width standard in AD, etc.

okhxyyo

bigbat posted on 2022-10-8 17:00 It is recommended that EEWORLD create a PCB standard process, such as the pin position of components, the symbol positioning of diodes, the board frame standard, vias, line width standards in AD, etc.

Good suggestion, I will look for information on this and see how to integrate it

wangerxian

Can the heat dissipation be done by drilling holes in the SMD pads?

LuJianchang

You can learn about the via-in-pad process, which is very suitable for BGA packaging

chunyang

This depends on how you solder. If you solder by hand, you can safely add vias to many surface-mount pads, but they must be exposed pads. When machine soldering small batches, you must pay attention to the package design and via size. When the number of pins is low, you can cautiously add vias after repeated experiments. For example, adding vias to the pads of the 0x0x RLC device has been proven to be feasible by experiments, but the pad size should be appropriately increased and the via diameter should be strictly controlled. The vias should be placed on the inner edge or outer edge in the length direction. At this time, even if it fails (the failure manifestation is often "tombstone"), it is easy to detect and correct it manually. Don't do this for large batches. It is easy to cause problems after manual intervention fatigue. However, for the package in the original poster's picture, it is not recommended to add vias, because it is difficult to handle once a problem occurs, and your via diameter is a bit too large relative to the pad size. The larger the via diameter, the more likely it is to cause problems.

Of course, in special cases, the problem can be solved by using a "plugging" method, but this will increase additional costs, including the cost of PCB production and quality inspection. "Plugging" is a process that solidifies the vias, and does not affect the soldering yield rate in batches.

For DIY, you can consider making the vias larger and manually filling them with tin before inserting the components. Of course, I have never done this, so I cannot guarantee the reliability, but I just think it is feasible.

chunyang

In my past designs, there are only two situations where surface mount pads are added with vias. One is multi-pin ICs such as LCC and SOP. It is completely fine to place the vias on the inner or outer edge of the pad, and it will not cause any problems for machine welding or even mass production. The other is RLC devices with a low number of pins. This is the solution mentioned in the previous post. In most cases, there is no problem. There is an occasional welding failure with a low probability, but there is no obvious difference in the failure rate compared with other similar pads without vias.

bigbat

okhxyyo posted on 2022-10-8 17:30 Good suggestion, I will look for information on this and see how to integrate it

My idea is: each topic has a title, and then everyone discusses and sorts it out.

秦天qintian0303

This depends on the situation. Some USB fixed pins may cause the pins to fall off when plugging and unplugging. In this case, they need to be fixed through vias.

btty038

Placing vias on pads can easily lead to solder leakage and short circuits. I have personal experience with this project and do not recommend doing so. If you cannot make way, it is recommended to cover the bottom with oil.

Reflow soldering is also likely to affect

okhxyyo

bigbat posted on 2022-10-8 18:34 My idea is: post a title for each topic, then everyone discusses it, and finally organizes it

I'll give you a little flower, brainstorming, this is really great. I think we can do it

qwqwqw2088

bigbat posted on 2022-10-8 16:28 This is a hard rule for me. There can’t be vias (>15mil) near the pads, and the copper connection also uses flower pads. Because I...

Yes, lead-free soldering is the most prone to problems

Be very careful when drilling the holes

qwqwqw2088

Via window, via cover oil, via plug oil

elec921

But lead-free is fine, the hole can be made smaller, 0.6/0.3mm, and hand soldering is not a problem