current
community

chat
blog

Electrical Engineering

Electrical Engineering Meta

your communities

Sign up or log in to customize
your list.

more stack exchange
communities

Stack Exchange

sign
up log
in tour

help

Tour
Start here for a quick overview of the site

Help Center
Detailed answers to any questions you might have

Meta
Discuss the workings and policies of this site

Electrical Engineering

Questions

Tags

Users

Badges

Unanswered

Ask
Question

Take the 2-minute tour
×

Electrical Engineering Stack Exchange is a question
and answer site for electronics and electrical engineering professionals,
students, and enthusiasts. It's 100% free, no registration required.

BGA
escape via dimensions at 0.8mm pitch?

up vote11down votefavorite

2

Are there any kinds of standards or common practice dimensions which
define what BGA escape vias and routing trace/space should look like at
0.8mm pitch? If not, what's the most economical set of dimensions to
use?

Several documents I found when searching online discuss vias and
routing dimensions on the top and bottom layers, but not inner layers. As
I understand it, the inner layers require antipad which makes them more
restrictive than the outer layers. Therefore these should be the driving
dimensions, but I can't find much on that.

I found a document BGA/PCB
Interconnect Design Guidelines that discussed 0.8mm pitch (search for
"0.8-mm"). It says that with a hole/antipad of 10/28 mil, only 3.5 mils
remain on the planes and that isn't good. It goes on to say that using
8/26 for hole/antipad still leaves only 5.5 mil, and so you should just
use microvias.

However, I see some manufacturers offer 8 mil inner clearance
(antipad?), so couldn't you use 8 mil holes with a 24 mil antipad and have
plenty of ground plane copper left?

I found this NXP document: PCB
layout guidelines for NXP MCUs in BGA packages. It has a nice but very
confusing table in it. It shows generally standard hole sizes like you'd
see from PCB manufacturers (12 mil, 8 mil, in mm) as drill size, and
finished sizes way way too small. The pad to drill size for 1mm pitch in
particular would be an entirely normal sounding 12/21 via but the
'finished size' is 7 mil! My understanding is that PCB manufacturers
operate on finished hole size, not drill size. What's wrong here? (or
with my understanding?)

pcb-design pcb-fabrication via

share|improve
this question

asked May 8 '11 at 3:42

darron
2,0781232

1

Your
PCB shop can work with either finished hole size or drill size.
Designs in my shop often specify "hole sizes 10 mil and smaller are
drill sizes. Hole sizes greater than 10 mil are finished sizes." Or
if we specify a finished size, we give enough tolerance that the
hole could be plated completely closed.
–  The
Photon May
11 '12 at 16:38

add a comment |

3 Answers 3

activeoldestvotes

up vote8down vote

+500

I'd love to say there is a simple answer, but there is not, there are
too many variables
However you can break the problem down.....

The sizes you select mostly depend on what the capabilities of the fab
you are using.
For low cost, reliability, and high yield choose the
largest vias and largest traces you can, while keeping annular rings as
large as possible and traces well spaced and as wide as possible.

Take a look at the capabilities of you chosen supplier(s) talk to them
and ask their advice, after all are the ones that have to guarantee they
can make it. e.g. Graphic's
Capabilities

Graphic PLC, like others, quote standard, low-yield and development
feature sizes.

More than anything else, your escape plan will also depend on the
parameters of your PCB.
How many layers do you need? How many rows to
you have to escape in your BGA? Generally you need (N/2)-2 layers, where N
is the largest number in the number of rows or columns in your BGA.
However, if you use microvias things get easier. Remember you don't
normally need to escape all the signals, GND and Power can often go direct
to the planes.

So, decide: Are using conventional vias, blind vias, buried vias,
microvias or microvia-in-pad?
The minium dimensions of the via drill
are partly controlled by the layer pair thickness (2:1 is a good starting
rule) plus type of PCB material. Harder, thicker materials means bigger
drills.
Are you using 18um or 36um copper, you might want the latter if
some other part of your circuit carries a high current or perhaps your
signal integrity rules play some part in you decision making process?
Bigger copper means more undercut which means more tolerance needed.

So first you need to decide what board construction you can stand given
your cost constraints in the volumes you are interested in buying, then
base your design constraints on that by looking at the capabilities of the
fab you want to use and the technology you require.

The reason manufacturers use finished hole sizes is that the drill
required is 0.1 to o.2mm larger than the finished hole size. So if you
want a 0.5mm finished hole, the manufacturer will drill it 0.7, then plate
it down to 0.5 with 0.1mm of copper. So the finished size seems small,
but a larger drill can be used.
Don't be so scared of small feature
sizes. You will be surprised just how small the drills can be, e.g.
Graphic can drill 0.15mm holes using a conventional drill if the material
is 0.2mm thick! However, smaller drills are more expensive as they break
more often so need replacing regularly (ideally before they break) As they
use more of them and being a bit trick, they cost more to replace.

The minimum size of the via pad is defined by the drill size and the
drill tolerance. Usually drill size (not finished size) +0.1mm is a
minimum. But that depends on yield and manufacturing tolerances.
Obviously bigger is better if you have room and you are not working at
10's of GHz.

Ok a worked example:
Using a 358 pin UBGA part, an Altera Arria
GX.

Looking at Graphic's data, I can select a 0.25 finished hole (i.e. 0.45
drill) with a 0.45 annular ring. I'll tent the top side.

Excluding power pins, I have 5 rows to escape. Ideally i'll need 4
layers.

Let's try without anything exotic (reducing cost)
vias 0.25 finished
0.45 pad
tracks 0.15mm, min gap 0.1mm
Stock BGA pads on library
symbol are 0.45 Not mask defined

That looks like this:

See we managed it on three of the 4 layers, and it looks like we can
still make some improvements; We could reduce the track and increase the
annular rings or go microvia-in-pad for reduced layer count.

share|improve
this answer

answered May 12 '12 at 15:54

Jason
Morgan
2,166415

I
should have included that the above gives you 0.15mm copper between
non-connected pads on the plane layers.
–  Jason
Morgan May
12 '12 at 16:04

Excellent
answer! –  Rocketmagnet
May 13 '12 at 20:18

@JasonMorgan,
Love the answer, I think a bit more formatting work might make it
look even snappier in google but you earned the 500, dont spend it
all in one place! –
Kortuk♦
May 17 '12 at 18:41

@kortuk,
Electronics and computers are my strong point yet I failed CSE
english - that probably shows. Thanks for the points!!
–  Jason
Morgan May
17 '12 at 19:36

@JasonMorgan,
Over the last 6 or so months this question is our top google hit, it
was number 2. I think the improved quality probably has more people
linking, thanks for writing this! Hope you decide to keep toying
with it when you get bored! –
Kortuk♦
Jun 2 '12 at 16:37

add a comment |

up vote0down vote

IPC7095B, which can be purchased here for $103, is worth buying. The price is negligible
compared to what you will be spending on your board design and PCB
manufacture.

IPC7095B
Table of contents

share|improve
this answer

edited
May 12 '12
at 9:41

stevenvh
111k9340560

answered May 8 '11 at 11:40

Leon
Heller
31.6k24071

2

Useful
document link is giving me a 404 error
–  ajs410
May 11 '12 at 20:27

add a comment |

up vote0down vote

The simple answer is, it depends which company your buyers use for PWB
orders on fine pitch parts.

Added: In my experience, a good buyer & engineer
with purchasing leverage in volume can get more significant cost
reductions {from qualified suppliers} by negotiation more than by design!
However if we are talking new design, baseline costs are usually unknown,
but I have seen and made deals like 10% off all std. fab. costs. just by
negotiation.

re: 0.8mm pitch BGA device layout recommendations, I offer the
following to discuss with your fabricator, if unsure;

Standard BGA design guidelines, IPC 6012B Class 2.

Drill Pad Anti-Pad PWB Ratio

6 16 26 39 6.5:1

8 18 28 62 7.75:1

10 20 30 100 10:1

12 22 32 120 10:1

14 24 34 135 10:1 units = 0.001" thick

Please note that most relevant "capabilities": "preferred" and
"minimum" trace width / spacing / via hole size / via pad diameter may
or may not affect product cost, but "minimum" generally implies lower
yields than "preferred" and hidden cost increases in quote will result.

IPC Design Guideline book is essential in your library as ref below. As
wel as close communication with your Board shop tech support.

share|improve
this answer

edited
May 14 '12
at 9:09

answered May 13 '12 at 20:21

Tony
Stewart
1

2

I
agree the IPC guide is a bible in the industry, +1 for that. It is
an excellent place to start if you are unsure. However personally, I
find it always slighty behind the techology used by the fab houses
in some areas so talking to them and understanding the reason behind
decisions is just as important. If you think about it, it's always
going to be the lowest common denominator, but that's not a bad
thing. –  Jason
Morgan May
17 '12 at 19:40

add a comment |

Your Answer

draft
saved

draft
discarded

Sign up or log
in

Sign up using Google

Sign up using Facebook

Sign up using Stack
Exchange

Post as a guest

Name

Email

discard

By posting your answer, you agree to the privacy
policy and terms
of
service.

Not the answer you're looking
for? Browse other questions tagged pcb-design pcb-fabrication via or ask
your own question.

asked

4 years
ago

viewed

4977 times

active

3
years ago

Related

0
Reducing
cost by eliminating microvias when designing a PCB with buried vias

1
0.5mm
Pitch BGA Fanout - Reasonable Vias, Drills, Traces and Clearances

2
PCB
vias impact in cost

10
Using
a via to strengthen surface mount connector on or near pad

1
Correcting
printed PCB (add a via)

2
PCB
Design: What is the minimum value of Via Dia and Via Drill size?

1
What
is the best way to plate VIAs?

1
How
do you change the default via dimensions in Altium?

4
How
to minimize characteristic impedance mismatches caused by vias?

0
Via
definition & routing on OrCAD - PCB Editor

Hot Network Questions

Calling the same method in two ways, big difference in
speed. Why?

Solve: Merging two branches of the solution

What are the restrictions imposed by the Sharia law in
Aceh, Sumatra?

Can I project a single set of coordinates that are not in a
table or feature class with arcpy?

Calculating an integral

Underwater spider webs made of slime?

Pathfinder Multi classing as a rogue archetype

What is the missing word?

Counting leap years

How to get Workflow Rule in Maven's Mate

Why did Voldemort take the wand of one of his most loyal
servants?

Is there a reason to believe that programming languages are
going to converge?

How do I set Notepad++ as an editor on Ubuntu?

Swapping click and middle click buttons

How did the Joker actually get his scars?

Changing PhD programs: should I submit a recommendation
letter from my old advisor if it's not purely positive?

My paper has not been published because I did not show up
for the conference presentation

Magento Events 'catalog_product_get_final_price' not
working?

Does case matters when reading and sorting a list of items?

What books address various difficulties that may arise
during various stages of meditation practice?

How to get Ctrl+Shift combination for Excel macro shortcut?

Google Webmaster Tools: duplicate title even with a 301
redirect in place

Temperature Converter

Firefox accusing me of distributing malware on my site

more hot questions

question feed

tour
help
blog
chat
data legal privacy
policy work
here advertising info
mobile
contact us
feedback

Technology

Life / Arts

Culture / Recreation

Science

Other

Stack
Overflow

Server
Fault

Super
User

Web
Applications

Ask Ubuntu

Webmasters

Game
Development

TeX - LaTeX

Programmers

Unix & Linux

Ask
Different (Apple)

WordPress
Development

Geographic
Information Systems

Electrical
Engineering

Android Enthusiasts

Information
Security

Database Administrators

Drupal
Answers

SharePoint

User
Experience

Mathematica

Salesforce

more (14)

Photography

Science
Fiction & Fantasy

Graphic Design

Seasoned
Advice (cooking)

Home
Improvement

Personal
Finance & Money

Academia

more (10)

English Language &
Usage

Skeptics

Mi Yodeya (Judaism)

Travel

Christianity

Arqade
(gaming)

Bicycles

Role-playing Games

more (21)

Mathematics

Cross Validated (stats)

Theoretical Computer
Science

Physics

MathOverflow

more (7)

Stack Apps

Meta Stack Exchange

Area
51

Stack Overflow
Careers

site design / logo © 2015 stack exchange
inc; user contributions licensed under cc by-sa 3.0 with attribution required

rev 2015.5.26.2605