Continue to Site

Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

polygon pour on top layer beneath BGA

Status
Not open for further replies.

rayhh27

Member level 1
Member level 1
Joined
Nov 22, 2016
Messages
34
Helped
0
Reputation
0
Reaction score
0
Trophy points
6
Activity points
361
Hi,

I am intending to design PCB using BGA IC, I am wondering whether is it not good if I use polygond copper right beneath the BGA package? Why?
Thank you.

Best regards,

RH
 

KlausST

Super Moderator
Staff member
Advanced Member level 7
Joined
Apr 17, 2014
Messages
23,048
Helped
4,716
Reputation
9,448
Reaction score
5,092
Trophy points
1,393
Activity points
152,683
Hi,

What BGA pitch is it to have that much space?

Klaus
 

KlausST

Super Moderator
Staff member
Advanced Member level 7
Joined
Apr 17, 2014
Messages
23,048
Helped
4,716
Reputation
9,448
Reaction score
5,092
Trophy points
1,393
Activity points
152,683
Hi,

give useful informations.

Klaus
 

rayhh27

Member level 1
Member level 1
Joined
Nov 22, 2016
Messages
34
Helped
0
Reputation
0
Reaction score
0
Trophy points
6
Activity points
361
Hi,

so it is like this there are many vcc, vccd_pll, etc. So like GND they are near each other and I am wondering whether it is ok to connect them using polygon.
If it is not enough what kind of information should i provide.

Thank you,

RH
 

marce

Advanced Member level 5
Advanced Member level 5
Joined
Feb 23, 2010
Messages
2,032
Helped
623
Reputation
1,248
Reaction score
615
Trophy points
1,393
Location
UNITED KINGDOM
Activity points
14,098
Do you mean power planes below the BGA, common practice, suppress inner layer lands but add 0.15mm overdrill if your system supports it to get the thickest web between vias.

Suggest you have a look at this...
**broken link removed**
 

FvM

Super Moderator
Staff member
Advanced Member level 7
Joined
Jan 22, 2008
Messages
50,813
Helped
14,603
Reputation
29,481
Reaction score
13,688
Trophy points
1,393
Location
Bochum, Germany
Activity points
290,949
The question title suggests you want to a copper pour connecting multiple adjacent BGA balls. That's surely possible.

A side effect is however that BGA pads inside a copper pour become larger than others because they are effectively solder mask defined pads. Usually that's no problem in reflow solder.

You see the effect with a BGA power IC (0.8 mm pitch) that has some pads on a copper pour:

BGA+copper pour.jpg
 

FvM

Super Moderator
Staff member
Advanced Member level 7
Joined
Jan 22, 2008
Messages
50,813
Helped
14,603
Reputation
29,481
Reaction score
13,688
Trophy points
1,393
Location
Bochum, Germany
Activity points
290,949
All BGA pads have nominal 0.4 mm diameter (NSMD), the isolated pads are actually etched down to about 0.35 mm. The pads inside a copper pour are effectively solder mask defined to nominal 0.5 mm, actually 0.57 mm.
 

FvM

Super Moderator
Staff member
Advanced Member level 7
Joined
Jan 22, 2008
Messages
50,813
Helped
14,603
Reputation
29,481
Reaction score
13,688
Trophy points
1,393
Location
Bochum, Germany
Activity points
290,949
Apart from PCB manufacturing tolerances (or possibly intentional modifications by the PCB house) visible in the example, it's exactly what you can expect when placing BGA pads on a copper pour (or traces wider than the pad).

I understood the original question so that the OP intends something similar, thus I showed this real world example to illustrate possible side effects.

In the present design, the copper pour is preferred to achieve low connection resistance for a switch mode regulator. I agree that the pad finish look curious, but I feel that it's still the best option in this case.
 

marce

Advanced Member level 5
Advanced Member level 5
Joined
Feb 23, 2010
Messages
2,032
Helped
623
Reputation
1,248
Reaction score
615
Trophy points
1,393
Location
UNITED KINGDOM
Activity points
14,098
Firstly I always follow the IPC 7351 recomendation of 1:1 for solder resist openings, allowing the manufacturer to open the resist enough to get a good yield rate but avoid solder resist encroachment on pads. When solder mask defined pads come into the equation even more care is needed both from the manufacturer and the designer. If not then you can suffer bad solder joints on you BGA due to the differences in pad sizes... Round BGAs the extra added to the solder resist opening should be pretty minor to avoid exposure of copper to avoid solder shorts.
 

Status
Not open for further replies.

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Top