3
\$\begingroup\$

I am currently designing an HDI-PCB. Outer-layers micro vias, inner layers buried vias.

As cost is of big concern my idea is to not fill and cap (copper plating) vias (100 μm drill ~ 75 μm finished diameter) in 0201 and 0.35 mm pitch BGA pads.

My reasoning is: As the outer prepreg (60 μm) and the copper film (30 μm after plating) are extremely thin (~90 μm) I do hope, that there is no issue in reliable soldering.

As a precaution I did place such a via in every BGA pad (so it does sit "in the pit"), as well as on every 0201 pad (not just a single pad per part were required).

My questions: How wrong is this assumption?

Are there any suggestions to minimize negative effects and still save the extra cost associated with via filling and plating (low quantities, so rather high PCB costs)?

Do you have any experience with such an approach (assembly yield, etc.)?

Why do I ask: I have read some articles and posts - these give me headaches. But, as these discussions do mostly focus on ~0.3 mm vias through 1.6 mm PCBs, I am still optimistic.

\$\endgroup\$
5
  • 3
    \$\begingroup\$ Have you asked your intended manufacturer? FWIW its fairly normal IME not to do via-in-pad for BGA pads. Your biggest cost adder is not the capping but the blind and burried vias \$\endgroup\$ Commented Aug 11, 2022 at 23:00
  • 1
    \$\begingroup\$ The added area needed to get rid of buried/blind vias will likely cost less than keeping things tight and using buried/blind vias. If you can avoid buried/blind vias, do so. Some products require the high density, so you may have no choice, but for prototypes and so on - buried/blind vias are a luxury unless you're prototyping the final layout - not always the best idea. \$\endgroup\$ Commented Aug 12, 2022 at 0:10
  • \$\begingroup\$ @crasic Hmmm BGA is 0.35 Pitch with 90/90um Track/spacing on outer Layer. It is only a 4x4 (16WLP) device - but routing without Via-In-Pad is out of question. \$\endgroup\$ Commented Aug 12, 2022 at 19:43
  • 1
    \$\begingroup\$ I am probably overloading a term. What I mean is that the forgoing the fill-and-cap process for vias in pad is on tight BGA breakout is typical in my experience. There are manufacturing process concerns e.g thermal conductivity and solder-ability. They are not insurmountable, recommend to engage the manufacturer early in your process. At the end of the day, you can imagine whatever design rules you would like, and the question is if it represents the capabilities of a real world manufacturing process. There is nothing inherently wrong with a via in pad that is not capped. \$\endgroup\$ Commented Aug 12, 2022 at 20:14
  • 1
    \$\begingroup\$ Also, keep in mind with small quantities it is much easier to QA or hand-pick the best production articles, question is if the potential reduction in yield and chance of scrapping a board exceeds the cost of simply going with the more reliable process, assuming it is more reliable, which would be up to the QA expert of the manufacturer to confirm, or someone with equivalent process know-how on your team. \$\endgroup\$ Commented Aug 12, 2022 at 20:22

1 Answer 1

Reset to default
2
\$\begingroup\$

You need a smooth, level surface to apply paste to your BGA and discrete pads. IPC spec allows for "dimples" in pads containing vias, but the maximum allowed depth of such a dimple is pretty small. A large "dimple" - such as what would effectively happen if you didn't fill the via - would trap air that could bubble out during reflow, compromising the integrity of your solder joints.

That said, I don't think you would be able to find a vendor that wouldn't fill those pads. 100 μm [4 mil] laser drill vias are almost certainly going to be 100% fully copper plated shut by your vendor as part of their standard process. In my experience, vendors will only opt to resin fill and cap laser vias above around 200 μm [8 mil] in diameter. You should of course talk to your specific vendor to understand their manufacturing processes.

Your buried vias, if of similar size, would also likely be electroplated shut as part of their standard process. If these were larger, such that they wanted to use a non-conductive resin fill, then they would do so but wouldn't cap them. (I think they would want to fill them, as the board could otherwise end up with resin starvation on the nearby prepreg layers after lamination, but there's no need to cap them as they are internal to the board and not in solderable pads.)

\$\endgroup\$

Start asking to get answers

Find the answer to your question by asking.

Ask question

Explore related questions

See similar questions with these tags.