Filled via and via in pad

[tszaboo]

I've a design, where one side of the board gets potted for many reasons. Because of this, after many trials the best course to avoid the potting compound to go to the other side of the board, via filling was decided. IPC4761 Type 7, if that tells it to someone. So this is new to me, so far I didn't do boards with this technology. I can place the via into a pad, very nice. For example a 0402 bypassing capacitor will be about the size of two vias, so the power can go directly there. It looks like a serious size saver, maybe even 50% on these parts. I actually starting to think that BGA is better suited for this. For example a QFN package will have pins that are 0.5mm apart and the pad is ~0.2mm wide, impossible to place a via, while QFN will just nicely take a via in each pad, smaller package with more space between the pins.
Do you have experience with this? What did you think the first time using it?

[tszaboo]

Anyone?

[Niklas]

Drilled vias usually gets filled and shut with solder mask if the drill diameter is 0.3 mm or less. From ow experience of mass production, 0.4mm are almost shut, but the second side printing can still flow through and form small droplets on the opposite side. Something to be aware of if the via is placed underneath a component.
Make sure you cover both sides of the via with solder mask in your design and state that they are tented/filled shut to the Pcb manufacturer.
I would avoid BGAs and potting as the potting could cause damage to the package and the solder balls during thermal cycling.

[brabus]

Yes, I have experience with this kind of design. Mine was a 6-layer, 0.5 mm thickness, HDI with SBU. Total dimension 18 x 36 mm, it integrated 5 BGAs with minimum pitch 0.40 mm.

The game changer, apart from having ViP (Via-in-Pad) is the SBU (Sequential Buildup): choose the sequence wisely in order to obtain maximum flexibility but also avoid exaggerated costs. For example, on a 6-layer, you can have blind vias 1-2 and 5-6, buried vias 2-5, plus the usual 1-6. This sequencing is not that much more expensive than the traditional 1-6, but it allows you to do pretty much anything you want on the board, e.g. placing two large BGAs face-to-face on opposite sides of the board.

If you are not going for SBU, filled and capped vias allow you some neat tricks, not to mention the freedom you can take with the soldermask: bye bye solder wicking!
On the thermal side of things I haven't noticed a huge improvement, but my design was not that challenging on this aspect.

[tszaboo]

So considering JLC will do very cheap via in pad PCBs I decided to try this for a personal project.
Its not what we use at work, but I've seen both companies do via in pad and they look similar.
You can place a standard size via in the pads of a 0402 capacitor, I highlighted it on the image. As I suspected, it makes bypassing capacitor layout sizes ~50% smaller. With double sided load, you can easily place two capacitors on two sides of the board, and with multilayer design they go directly into planes. I really like the concept.

Drilled vias usually gets filled and shut with solder mask if the drill diameter is 0.3 mm or less. From ow experience of mass production, 0.4mm are almost shut, but the second side printing can still flow through and form small droplets on the opposite side. Something to be aware of if the via is placed underneath a component.
Make sure you cover both sides of the via with solder mask in your design and state that they are tented/filled shut to the Pcb manufacturer.
I would avoid BGAs and potting as the potting could cause damage to the package and the solder balls during thermal cycling.

I don't think that's the Type 7 via closing. 7 is filled with epoxy, and completely closed on both sides with copper plating over.

Yes, I have experience with this kind of design. Mine was a 6-layer, 0.5 mm thickness, HDI with SBU. Total dimension 18 x 36 mm, it integrated 5 BGAs with minimum pitch 0.40 mm.

The game changer, apart from having ViP (Via-in-Pad) is the SBU (Sequential Buildup): choose the sequence wisely in order to obtain maximum flexibility but also avoid exaggerated costs. For example, on a 6-layer, you can have blind vias 1-2 and 5-6, buried vias 2-5, plus the usual 1-6. This sequencing is not that much more expensive than the traditional 1-6, but it allows you to do pretty much anything you want on the board, e.g. placing two large BGAs face-to-face on opposite sides of the board.

If you are not going for SBU, filled and capped vias allow you some neat tricks, not to mention the freedom you can take with the soldermask: bye bye solder wicking!
On the thermal side of things I haven't noticed a huge improvement, but my design was not that challenging on this aspect.

I would love to do blind and buried vias, but nothing I designed called for that so far. And I agree, it's not that expensive for small boards, but for example the last one I designed (not this) was ~130 x 70 mm, and there wasn't really a need to make it smaller, because the rest of the device is big, and Antennas wouldn't work properly with smaller sized boards.

[tszaboo]

And here is the board ordered. It's amazing how much you can place in a very small PCB.

[ejeffrey]

Yes, plugged and plated over vias are great.  Not only do they really improve density, but they reduce inductance and make your bypass capacitors more effective at high frequency.

The big thing to watch out for is losing your test points.