BGA IC board design

"Thiago" <thiago_hr@yahoo.com.br> wrote:

Hi, could someone please provide me a board design sample with a BGA

IC so I

can check how it is done? I´ve never designed a board with suck

package, and

I have some doubts about it.

http://www.xilinx.com/support/documentation/application_notes/xapp489.pdf

Here are some examples. The cheapest way is to put normal vias between

each ball. The more expensive is microvias IN the pads. Some

manufacturers can fill outer layers with copper so that 'normal' vias

can be put ON the balls.

There is nothing to worry about as long as you use a manufacturer that

can do the density that it requires. Ive done it a lot with Eagle.

In article <1440662276307224458.579862mleikvol-

yahoo.nospam@news.cadsoft.de>, mleikvol@yahoo.nospam says...

 

"Thiago" <thiago_hr@yahoo.com.br> wrote:

Hi, could someone please provide me a board design sample with a BGA

IC so I

can check how it is done? I?ve never designed a board with suck

package, and

I have some doubts about it.

 

http://www.xilinx.com/support/documentation/application_notes/xapp489.pdf

 

Here are some examples. The cheapest way is to put normal vias between

each ball. The more expensive is microvias IN the pads. Some

manufacturers can fill outer layers with copper so that 'normal' vias

can be put ON the balls.

There is nothing to worry about as long as you use a manufacturer that

can do the density that it requires. Ive done it a lot with Eagle.

Thanks, it is a nice ideia... but I am having a hard time placing vias

between the ball pads... my BGA has 0.8mm pitch and 0.3mm balls

diameter. My PCB manufacturer requires 0.2mm Drill... but the via still

has a ring too big to fit between the pads...

"Thiago" wrote

Thanks, it is a nice ideia... but I am having a hard time placing vias

between the ball pads... my BGA has 0.8mm pitch and 0.3mm balls

diameter. My PCB manufacturer requires 0.2mm Drill... but the via still

has a ring too big to fit between the pads...

>

The manufacturer will specify the minimum drill diameter for the via and the

min width of the copper around the hole.

You change the width of the copper around a via drill hole using the

"restring" setting in the DCR. (DRC/Restring)

Now you have vias in clear space between the balls you then need to ensure

you have a "clearance" to the balls that is greater than the minimum

distance requirements set in the DRC/Clearance for 'different' signals

HTH

Warren

"Thiago" wrote

Thanks, it is a nice ideia... but I am having a hard time placing vias

between the ball pads... my BGA has 0.8mm pitch and 0.3mm balls

diameter. My PCB manufacturer requires 0.2mm Drill... but the via still

has a ring too big to fit between the pads...

>

The manufacturer will specify the minimum drill diameter for the via and the

min width of the copper around the hole.

You change the width of the copper around a via drill hole using the

"restring" setting in the DCR. (DRC/Restring)

Now you have vias in clear space between the balls you then need to ensure

you have a "clearance" to the balls that is greater than the minimum

distance requirements set in the DRC/Clearance for 'different' signals

HTH

Warren

warrenbrayshaw wrote on Tue, 28 September 2010 17:48

"Thiago" wrote

Thanks, it is a nice ideia... but I am having a hard time placing

vias

between the ball pads... my BGA has 0.8mm pitch and 0.3mm balls

diameter. My PCB manufacturer requires 0.2mm Drill... but the via

still

has a ring too big to fit between the pads...

>

 

The manufacturer will specify the minimum drill diameter for the via

and the

min width of the copper around the hole.

You change the width of the copper around a via drill hole using the

"restring" setting in the DCR. (DRC/Restring)

 

Now you have vias in clear space between the balls you then need to

ensure

you have a "clearance" to the balls that is greater than the minimum

distance requirements set in the DRC/Clearance for 'different' signals

You can certainly get EAGLE to handle BGA's--I have 4 of them on the board

I'm currently working on.

Here's what I do to start with BGA's.  Once you have the infrastructure

right the rest is much easier:

1)  Add BGA device to the schematic (added to the PCB automatically)

2)  Go to PCB and set grid to be 1/2 of the ball grid pitch (so 0.4mm for

0.8mm-pitch BGA).

3)  Move the BGA package but hold down the CTRL key (CMD in MAC) so that it

snaps to the current grid.  Doing this now means that when you place the

vias they will be exactly at the center of the space which gives you the

most margin.

4)  Now add a few vias of the size you intend.  Run the DRC.  If there are

errors either change the via size or the Via rest-ring setting in the DRC.

Iterate until you don't have any DRC errors.  Doing this smartly will give

you the loosest manufacturing requirements to meet your design needs.

5)  Now route a trace of the minimum width you are allowed with your

manufacturing process to make sure it won't give you a DRC error when

routed through the grid array.

If you get that far then you have the settings that you'll need to use.

When routing out of the BGA always change to that grid to place the via and

it will be perfect every time.  EAGLE 5's "grid last" command is handy for

this.

Also, if you ever have to move that section of the circuit make sure you

move it by a multiple of the BGA grid so the vias stay on grid.  If it ever

gets off it's way harder to deal with--trust me, I know.

Hope that helps.  With this approach I have successfully laid out many,

many boards that have BGA's on them.

James.

--

James Morrison  ~~~  Stratford Digital

Specializing in CadSoft EAGLE

• Online Sales to North America

• Electronic Design Services

• EAGLE Enterprise Toolkit

--

Web access to CadSoft support forums at www.eaglecentral.ca.  Where the CadSoft EAGLE community meets.