15
\$\begingroup\$

Once I mistakenly placed a via on 0603 pad and didn't have any problem on soldering. I am routing another board now and I could save some space by placing some vias (0.3mm) on a 0603 pad. I wonder if it is a used technique or is it a bad practice? Would it cause PCB or PCBA production, or performance problem?

The via connections are low frequency (max 1.2 kHz) and related connections looks like this. enter image description here

\$\endgroup\$
  • 5
    \$\begingroup\$ I have seen this at some places to make debugging harder \$\endgroup\$ – PlasmaHH May 12 '15 at 19:21
  • \$\begingroup\$ I would expect it to be more of a soldering problem, but if you do it by hand and are not soldering BGAs, that should be fine. \$\endgroup\$ – Nazar May 12 '15 at 19:22
  • \$\begingroup\$ @PlasmaHH Do you mean reverse engineering? \$\endgroup\$ – Spehro Pefhany May 12 '15 at 19:27
  • 1
    \$\begingroup\$ @SpehroPefhany: That was probably the original intention of the engineer ... \$\endgroup\$ – PlasmaHH May 12 '15 at 19:31
29
\$\begingroup\$

The industry term for this is via in pad.
It's not a problem when you hand-solder components.
It can cause problems during automated SMT assembly. Solder, which was applied to the pad as a solder paste, can drain through the via and there will be an insufficient amount of solder to hold the part.

enter image description here
(Image came from this blog entry, which illustrates the issue.)

There are methods in which the via in the pad is filled with solder or epoxy. That is done prior to SMT assembly. That adds to cost of assembly, so the benefits from the via-in-pad need to justify that.

Related

older thread: Vias directly on SMD pads
article: Via-in-pad guidelines for PCBs

\$\endgroup\$
  • 1
    \$\begingroup\$ For best hand soldering place a kapton tape on the other side. \$\endgroup\$ – Gilad May 12 '15 at 21:06
  • \$\begingroup\$ To add to this, if you send it off for manufacturing; via-in-pads are mind-numbingly, insanely expensive. \$\endgroup\$ – ARMATAV May 13 '15 at 4:56
  • 1
    \$\begingroup\$ To resolve this, the solder stencil can sometimes be modified to account for this. In some cases it merely needs a bigger aperture for more solder paste, but in some cases (bga via-in-pad, for instance) the solder mask is actually thicker (ie, CNC machined in all three dimensions) so that more solder paste is applied at particular pads. Easiest and often cheapest, though, is to pre-fill these vias during fabrication, or sometimes with a solder stencil and oven process before putting parts on the boards. \$\endgroup\$ – Adam Davis May 13 '15 at 13:38
13
\$\begingroup\$

There's nothing wrong with via in pad per say. As other people have noted an open via in pad can lead to soldering issues as the solder is sucked down the via hole. Hand soldering you'll be fine of course, also for small runs the manufacturer can just pre-fill the hole with solder by hand with an iron or a hot air pen. This usually eliminates most of the aforementioned issues.

Doing it with a BGA can be funny, or sad depending on if it's your board or someone elses. The vias like to wick all the solder from the balls right to the back of the board, or at the very least make just one critical ball have a bad or weak contact. That's nice when that fails in the field 3 months later :)

For real production again, nothing wrong with via in pad, it's really useful in many cases. All you have to do is have your pcb shop fill the holes. I usually let them fill with non-conductive material and then plate flat so we end up with a solid metal flat pad to solder to. There's a little cost adder for this but really it's not that bad.

Just another trade off you have to make to see if you can afford the extra cost.

\$\endgroup\$
  • 1
    \$\begingroup\$ Just an addition to above: you can fill vias yourself with solder paste; just print once without stencil (masking PTH holes first if you still use them). The trick is called 'stuffed vias" in boardhouse lingo. \$\endgroup\$ – Oleg Mazurov May 12 '15 at 20:49
8
\$\begingroup\$

Great answers from others but for completeness I'd add two cases where via in pad can be used for good effect.

  1. Mechanical strength in the z-axis of a pad. You'd use it in surface-mount connectors where you want to add some robustness. It acts a little bit like a rivet and helps prevent the connector from lifting. I used this many times, particularly on SMD USB connectors that get quite a bit of hammering and torque from the cable head. You don't have to put a pad underneath, but sometimes I'll do that too if I have the space. Just make sure that the amount of bolting vias per pad is the same. EDIT: found this question about this very technique!

  2. Syphoning solder in large pads, like those under the large ICs. This helps against the chip 'floating' on a melted solder blob -- not soldering the pins! -- in case your stencil or dispenser allowed for excessive amounts of solder on the pad.

\$\endgroup\$
5
\$\begingroup\$

I did this once thinking I was being smart, and what happened is that all the solder wicked off the pad and through the via onto a test point on the other side during reflow soldering. Had to hand solder all the connections until I re-did the board.

If you are soldering the boards by hand then there should be no problem, and you can probably get away with it if the via is very small and there is no pad on the other side, but otherwise I would advise you to avoid doing this.

\$\endgroup\$
4
\$\begingroup\$

Placing a via on or very near to a pad can result in a weak connection or even tombstoning due to the solder being pulled away during reflow. It is recommended to have a small amount of solder mask between the pad and the via in order to prevent this from happening.

\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.