> James Nick Sears wrote:
>> Hi,
>>
>> I'm thinking about making the jump into a 256 pin BGA for my next
>> project, but I have a lot of unknowns when it comes to actually doing
>> the layout.  Does anyone have a good reference for things like what
>> sort of footprint to use (a grid of vias, right?)
> Generally no! Via-in-pad is possible but only with very specialist PCB
> processes. If you try to do it with ordinary sized unfilled holes it
> will just suck the solder away. Normal practice is to leave the pad
> diagonally and then via down to an internal layer.
>
> The footprint itself should be a simple grid of (generally round) pads.
> For details on the size and spacing of pads check with the manufacturer
> of the device in question.
>
> You will need a PCB process fine enough that with vias positioned as
> above you can get at least one and preferablly two tracks on each layer
> between a pair of vias. For a 1mm fineline BGA to get two tracks between
> a pair of vias you will want something like .1mm track gap and annular
> ring and .3mm holesize.
>> , suggestions on
>> routing all of those pins out into the open
> For the power pins you probablly want to go straight into an internal plane.
>
> For the signal lines it depends how much space you have, if you have
> loads of space try to route out to the side nearest the pad in question.
> If space is tight you will just have to add layers and/or reduce feature
> sizes until the tracks fit in the direction you want.
>
> Blind vias are also an option but I suspect they will considerablly
> drive up costs. If using them you want to route the pins from the middle
> of the chip on the lower layers.
>
> If working with an fpga it is often usefull to switch pins arround as
> you find which pin is easiest to get to for each track.
>
> If the chip has a load of power/ground pins in the middle then by
> carefull positioning of the vias you may be able to squeeze in some caps
> under the middle of the chip.
>
>