Connect with us

BGA-272 and double side PCB

Discussion in 'CAD' started by eeh, Mar 30, 2005.

Scroll to continue with content
  1. eeh

    eeh Guest

    I want to ask a question:

    I am doing a project which needs a DSP chip with BGA package. It has
    272 pins. Is double layer PCB enough for routing?

  2. Leon Heller

    Leon Heller Guest

    You'll need at least six layers!

  3. 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

    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.

  4. Guest

    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!
  5. Kunal

    Kunal Guest

    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.
Ask a Question
Want to reply to this thread or ask your own question?
You'll need to choose a username for the site, which only take a couple of moments (here). After that, you can post your question and our members will help you out.
Electronics Point Logo
Continue to site
Quote of the day