Vias on the pads of a BGA.

[luiHS]

 
I'm starting to work with BGA, and today reading the datasheet of a chip that acts as a MIPI switch, the PCB layout example caught my attention. Apparently they are putting vias on the BGA PCB pads. I had not seen this before in any general BGA PCB design documentation.

Is it recommended this way of putting "vias" or does it have any inconvenience and can cause problems?

I have some designs to do with an STM32H7 that will have quite a few tracks to route on a 240 ball BGA, and it might be difficult to get all the tracks out from inside the pads. If I can put vias directly on the pads I think it would be easier.

[SiliconWizard]

The inconvenience is that it requires a specific capability for the PCB manufacturer (called via-in-pad) which will plug vias in the pads *and* arrange to have as flat finish as possible over them. This is expensive.

[Psi]

Usually they fill them up and then plate them over the top with copper, sometimes called 'capped'
So they look like a normal pad with no via, but there is a via hidden under the surface.

[DavidAlfa]

Needs to be buried blind vias, filled with conductive epoxy and plated afterwards, usually pretty expensive!
Normal via is a bad idea, the hole will suck some of the solder and create lots of headaches.
A basic pcb design rule is to never put vias on smd pads.

https://www.pcbgogo.com/blog/What_Is_Via_in_Pad_.html

If possible, put the smallest via between the pads, ex.:


Otherwise that pcb is going to be really expensive!

[luiHS]

Thanks to everyone for your replies.
I contacted the JLCPCB and they told me that they do make vias in pad, but it is only free of charge for 6-layer boards.

https://jlcpcb.com/help/newsdetail/019666d056614efca51a965283c90751/86e689fe1363412d9ae61002e3de27f6

For those with 4 layers, they would have an additional cost that is not calculated automatically when ordering, you have to leave it in comments and they will respond with the real cost.

When I make my designs with the STM32H747X, I'll see if I find it interesting to make 6-layer PCBs and use vias in pad to facilitate routing. I have to route a lot of tracks from that chip to connect an external parallel SDRAM among other things, and I guess it will be tricky.

[SiliconWizard]

Thanks to everyone for your replies.
I contacted the JLCPCB and they told me that they do make vias in pad, but it is only free of charge for 6-layer boards.

Wow, I didn't know they did and especially free of charge. 6-layer is reasonable for high-density PCBs with fine-pitch BGAs anyway. Now wondering about the quality, if someone has any experience with them.

[uer166]

I contacted the JLCPCB and they told me that they do make vias in pad, but it is only free of charge for 6-layer boards.

What? That's awesome news! Does JLC charge same price as others for similar spec 6-layer or is it more $$.

[redkitedesign]

When I make my designs with the STM32H747X, I'll see if I find it interesting to make 6-layer PCBs and use vias in pad to facilitate routing. I have to route a lot of tracks from that chip to connect an external parallel SDRAM among other things, and I guess it will be tricky.

Well, theoretically you should be able to fanout any 240pin BGA in 3 routing layers (when 1 of them is the mounting layer), it would probably be unwise to try and do it on a 4-layer board. 6-layer is a reasonable minimum, especially if you want proper power and ground planes (which will greatly enhance the performance of your SDRAM interface). Depending on the density, an 8 layer board could be reasonable too.

Depending on your future plans with the design, I might not want to use the "free" via in pad from JLPCB. It might lock you in to this vendor, and you might want to have options to shop with the design for later production runs.

If its a one-off, I would totally go for it!

[voltsandjolts]

Needs to be buried blind vias, filled with conductive epoxy and plated afterwards, usually pretty expensive!
Normal via is a bad idea, the hole will suck some of the solder and create lots of headaches.

Hmm, I'm not so sure. I've been meaning to try out just using (small) standard vias and prefill with solder before BGA attach. Of course you would not do this for a production run but for a few hobby/proto boards I think it has a fair chance of working.

[woofy]

Dave has done a video on BGA fanout:
https://youtu.be/_1dr5FWYDgE

[DavidAlfa]

Ah, yeah, if you manually do that it'll probably work fine.
Couldn't know the target, thought it was professional, filling BGA pads in 1000s of boards for a commercial product seems like a PITA.

[wraper]

How are you supposed to fill those vias with solder in a way they stay flat? If you later try to clean them with solder wick, it will remove the solder from vias too.

[DavidAlfa]

Given you're already willing to hack the limits, you could achieve it under the cheap standard 4-layer tolerances by:
- Using 0.8mm pitch BGA (0.5mm/0.65mm will be a PITA with the vias)
- Using the smallest via diameter: 0.4mm pad, 0.2mm hole
- Hacking the BGA bads from 0.4mm to 0.33mm to provide the required 0.2mm clearance between via outline and pads/traces.

I don't think downsizing the pads down to 0.33mm will cause any problem, and jlcpcb shouldn't charge any extra for non-standard fab rules.

[SiliconWizard]

Needs to be buried blind vias, filled with conductive epoxy and plated afterwards, usually pretty expensive!
Normal via is a bad idea, the hole will suck some of the solder and create lots of headaches.

Hmm, I'm not so sure. I've been meaning to try out just using (small) standard vias and prefill with solder before BGA attach. Of course you would not do this for a production run but for a few hobby/proto boards I think it has a fair chance of working.

Uh, yeah. I don't think so.

[Psi]

Needs to be buried blind vias, filled with conductive epoxy and plated afterwards, usually pretty expensive!
Normal via is a bad idea, the hole will suck some of the solder and create lots of headaches.

Hmm, I'm not so sure. I've been meaning to try out just using (small) standard vias and prefill with solder before BGA attach. Of course you would not do this for a production run but for a few hobby/proto boards I think it has a fair chance of working.

You might get that to work with those multi-row QFN chips that have solid metal plugs instead of balls.
But with a solder ball BGA you will find it tricky.  Not impossible, but pretty hard.

[voltsandjolts]

For small pinout BGAs it might just work.
I glanced at the picture in the OP and saw the 36-BGA, but now realise the OP is actually talking about 240-BGA.
So, yeh, my possible cheapskate method is not relevant here.

[JPortici]

FYI JLC is currently offering a huge discount on 6-layer, up until the first half of january
makes me want to try designing/building one of jay carlson's boards for myself