BGA-272 and double side PCB

If you need a DSP then presumably you need it because it needs to crunch numbers. In that case you're going to need a good power and ground plane and power distribution network. So two layers is certainly not enough.

The number of layers you'll need depends on how the 272 balls are configured on the package and how the signals go to those balls.

Analog devices has a 576-ball BGA in which there are only I/O signals on the outer 4 layers around the outside of the BGA. The inside is all ground and power pins. This makes breakout much easier. I was able to lay that out with 4 signal layers. It could have been done with

2-layers with a few of the system requirements relaxed.

Other determining factors are what trace widths and separation rules you can use/afford with your board shop and the pitch of the 272 balls, the size of the overall board assembly, the pitch of the BGA balls, the via drill size, the annular ring size, ....

If you could route the signals on two layers then at a bare minimum you'll need 4-layers. I would imagine that will more than likely become

6-layers and quite possibly 8-layers. The board I did with 4 layers of routing also had 4 layers of power/ground planes for a total of 8.

Take this as a reference only. Without knowing the rest of the details I can only speculate. YMMV.

Cheers.

You'll need at least six layers!

Leon

I agree with Leon.

2 plane layers : Power and Ground and 4 signal layers.

The number of layers depends on the number of rows deep of the BGA you want to tap into. Top layer : 2 rows\\ next inner layer : 2 more rows every subsequent signal layer : 1 more row.

So first decide the number of rows you want to dig into and then calculate the number of layers. Dont count the power/ground pins for this since they will directly connect to the plane layers with vias.

Read applicatio notes on Xilinx and Altera about BGA layout. It is tricky, dont do it unless you are certain.

TIP: Make sure the feedthrough vias near the BGA pads are tented. Else the solder paste can get sucked into the via.

On Wed, 30 Mar 2005 16:22:12 -0500, James Morrison wrote:

You need to consider all of that, plus the characteristic trace impedance and termination strategy. Also power plane decoupling. I would not ever try this on a two layer board, plus I would thrash an engineer who suggested it!