Smallest ball pitch on JLCPCB 4-layer

[ezalys]

What's the smallest ball pitch on a BGA part you've had success with on JLCPCB's 4-layer process? The 3.5/3.5 rule seems generous enough, but I worry about the minimum solder mask sliver. Sometimes the solder mask consistency leaves something to be desired. Any experience to share?

[DavidAlfa]

I'm also searching examples for this.
There's a huge cost increase going from 0.45 to 0.4mm vias.

[asmi]

The smallest I ever done with them was 0.8 mm, but I'm sure they can go lower. It's not that expensive to just try and see what happens.

[SMdude]

This is a 0.5mm pitch bga that I had done by JLC about a year ago.
I did have to modify the footprint a little so I could rout out without clearance issues, but it worked. I don't think I had to pay a fortune for it either, cost $150 for 15 panels 180x200 4 layer gold plate.

[Harjit]

I think (don't know) it will be 0.4mm. I'd asked (on EEBlog) about break out for 0.4mm ball pitch and people generously provided information and that makes me think it is possible.

You cannot do vias in the ball array. You can only escape one layer. I don't know about via in pad. I had planned to place "dots" of soldermask between the middle of four balls but I don't think I can get soldermask between balls.

[cgroen]

I do 0.4mm WLP (MAX77839) with JLC (for prototypes at the moment). So far everything has gone smooth. Its an awful small package, and it only works because of the simple routing.
The smallest "real BGA" I have done is 0.6mm pitch, that worked out well too from JLC

[DavidAlfa]

This is a 0.5mm pitch bga that I had done by JLC about a year ago.
I did have to modify the footprint a little so I could rout out without clearance issues, but it worked. I don't think I had to pay a fortune for it either, cost $150 for 15 panels 180x200 4 layer gold plate.

What's the trace width? Seems thinner that 5 or 3.5th.

[48X24X48X]

Do you guys think it's okay to up the recommended pad size of 0.23 mm by TI to the minimum of 0.25 mm by JLCPCB manufacturing limit?
TI has a lot of these DSBGA that has 0.4 mm pitch and 0.23 mm pad. Of course by right, they can't make it.

[thinkfat]

What's the smallest ball pitch on a BGA part you've had success with on JLCPCB's 4-layer process? The 3.5/3.5 rule seems generous enough, but I worry about the minimum solder mask sliver. Sometimes the solder mask consistency leaves something to be desired. Any experience to share?

The minimum solder mask sliver is 0.1mm. I derived that from the 0.05mm mask expansion and the 0.2mm minimum pad distance (for green mask) they specify. They will also remove solder mask between pads if its too thin, so if you rely on a specific mask bridge to be there it's better to confirm with them beforehand.

The solder mask quality on their 2-layer process is not good, in my experience. I have no complaints yet with the 4-layer process.

[thinkfat]

Do you guys think it's okay to up the recommended pad size of 0.23 mm by TI to the minimum of 0.25 mm by JLCPCB manufacturing limit?
TI has a lot of these DSBGA that has 0.4 mm pitch and 0.23 mm pad. Of course by right, they can't make it.

Maybe you can work around that with negative solder mask expansion, so that the pad is defined by the solder mask instead of copper? Not sure if JLCPCB will do it, though. They want 0.05mm positive expansion, but that's only due to their registration precision, they want to make sure the mask doesn't cover the pad. However, with pads defined by solder mask this is exactly what you want, so maybe you can negotiate that.

[cgroen]

I do a lot of designs with a package from Maxim with 0.4mm pitch and pads with 0.25 mm diameter. Works perfect every time from JLCPCB (including stencils for it)
(sorry for the not too great photo of the board ....)

[kayvee]

I have recently done two different boards with 0.5mm pitch u-blox SiP modules using their unmounted stencils without any issues.

[mon2]

Not to be a Debbie Downer but in my opinion, it will be best to review your PCB layout of this fine pitched component. Specifically see if your PCB layout will require via-in-pad services. If yes, then JLCPCB will be out of the running as your PCB shop. This will turn your design into a HDI processed PCB. The pricing for such HDI PCBs varies with the wind. For a small batch of HDI PCBs we recently designed, we had quotes from $600 to $1800 USD out of China for the same qty (30 pcs I believe). Our email box was flooded with offers out of China and some even phoned us to follow up. The variance in pricing was amazing.

We selected the lowest offer which was from Kingford PCB, Shenzhen who did not treat our via-in-pad PCB layout as anything special. This was for a 0.4mm ball pitch WLCSP device onboard. Just a FYI..

[48X24X48X]

Not to be a Debbie Downer but in my opinion, it will be best to review your PCB layout of this fine pitched component. Specifically see if your PCB layout will require via-in-pad services. If yes, then JLCPCB will be out of the running as your PCB shop. This will turn your design into a HDI processed PCB. The pricing for such HDI PCBs varies with the wind. For a small batch of HDI PCBs we recently designed, we had quotes from $600 to $1800 USD out of China for the same qty (30 pcs I believe). Our email box was flooded with offers out of China and some even phoned us to follow up. The variance in pricing was amazing.

We selected the lowest offer which was from Kingford PCB, Shenzhen who did not treat our via-in-pad PCB layout as anything special. This was for a 0.4mm ball pitch WLCSP device onboard. Just a FYI..

No, I don't need the via in pad capability. It looks exactly like what @cgroen board's layout completely where all the pin traces can get out directly. Not sure if both Maxim and TI used same layout for their power management IC but the layout is 100% same. I think I will give it a try.

[Kasper]

0.4mm bga from JLC, soldered in a $20 toaster oven with no solder paste, just a bit of flux.  Worked for my quick test board.

I think I ran almost 1A through that bga.

I only needed 2 layers but ordered 4 layer to get the tighter capabilities.

I think I used SMD (solder mask defined ( solder mask on top of bga pads)) pads with 0.25mm dia exposed copper pads

[suarezvictor]

This is the best example I can find for 0.5mm ball pitch
Do you remember the exact parameters used? Pad size, clearance, track width