Fanning out a 0.4mm BGA with 0.23mm ball diameter



I am tryin to fan out this What would be the PCB requirements for fanning out something like this? Do I need via-in pad and 4mil trace width? What would be the minimum via hole width I would need to fan this out(also how many PCB layers?)


For this chip. Due to the way they have laid it out even 4/4 is pushing things a little. If you use there recommended land pattern. You end up with a 7 thou (0.17mm) gap between pads meaning its more like 3/3.

For the vias. You have 0.23mm pads. Meaning you where already planning to pay for vias around this size. I would say go with a dogbone pattern for the center columns of pads. There looks to be sufficient space


No getting around this, at this density you are facing using a high end and relatively expensive pcb fab.
A 0.23mm diameter pad and 0.05mm max silkscreen excess around the pad on a 0.4mm pitch means 0.17 mm between pads. This is 6.69 mil so you would need a 2/2 process to route tracks between pads as shown in the TI datasheets


I assume you meant solder mask not silk screen here.


From the datasheet:


To clarif , I need a process where the size of the via hole + annular width on either size is 0.23mm? So via hole is about 0.1m, annular width is 0.05mm ?


I think we can’t help you far with that. Call your favourite PCB manufacturer and ask him for their HDI capabilities and rules. With via in pad you might also consider via plugging and overplating as well. For prototyping it might work without but you should have some x-ray on hand to verify if you have excess voids in that case.

You also have to think about whether you can layout with staggered vias or you have to pay for stacked vias. Keep in mind that the aspect ratio for microvias (independent of plugging) is 1:1. So you might rethink about the thickness of your outer dielectric.

Best regards, Martin


You have 0.33mm between pads diagonally, so there is possibly space for vias between the pads


To reiterate what @mla has said, you want to verify your design meets your target board house capabilities up-front. Once you have successfully fab’ed the boards once, then it is usually than easier to shop around. I have used Sierra Circuits on the first cut of HDI boards in the past because they have an free online HDI stackup planner and DFM tool to analyze your Gerbers. (No affiliation, etc.) You can use the tools without having to get a quote, if I recall correctly.


This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.