[PCB_FORUM] Re: 0402 round pads
- From: "Ooi, Ching Leong" <ching.leong.ooi@xxxxxxxxx>
- To: <icu-pcb-forum@xxxxxxxxxxxxx>
- Date: Wed, 10 Jan 2007 08:25:05 +0800
Hi,
ALIVH = Any Layer Inner Via Hole,
believe Panasonic or a Japan company (could not recall) holds a patent on that
. That PCB Fab process comes quite differently, they use build up technology
where PCB Fab starts with bare core , laser drilled and plated on and so on.
Cost impact probably comes in economic of scale (Qty), not just drilling alone
like typical PCB process where drilling time is the bottle neck that determine
the cycle time . But as of recent years clocking speed is going higher and RF
analogue becomes key integral part of design, couple with the madness of
miniaturization Every mil of trace count with every square mil of real estate
occupied, and that would have drive the adoption with cost justification.
Use of some techology via that tied some filter cap almost directly to ground
has some performance advantage, on higher frequency domain, effective coverage
of range of bypass/filter capacitor is very short , so designer resort to
placing them close or under BGA to ensure its effectiveness. Some even resort
to placing them surround the plane to ensure the power plane to it is well
clean up before goes to supply major chipset. stub is a definte "No". . I ain't
not expert so not able to comment a lot on that ...
Square pad seems to be favorite shape to use, I have seen rounded corner one
before ,cannot really tell the performance difference , but most important
factor, keep this two shape almost equal in area, because the copper detemine
the heat mass during reflow, or apply proper relief shape such that the heat
absorbed by the 2 pads is even. That would have cut down extent of unevenness
in thermal dissipation that leads to tombstone. Tombstone occurs when one side
of solder melts a little faster than another pulling the chip into standing
position.
my 2 cts,.
CL
________________________________
From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Gene Carman
Sent: Tuesday, January 09, 2007 5:49 AM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: 0402 round pads
Tell those "some folks" that the cell phone industry lives on those microvias
and cheap PWBs. I believe that the video recorder industry is a heavy user of
microvias and even uses ALIVH type vias.
Point those "some folks" to the internet where they can do a quick search and
read documents with words such as these: "Naturally however, economic
considerations for or against play a significant role. A comparison of variable
drilling costs reveals the superiority of microvia technology over mechanical
drilling (Ø 0.3 mm) even with a relatively small number of holes. The 100x
faster drilling speed and the tool costs approaching ZERO make laser drilling
extremely fast and cheap. This effect becomes more pronounced as the number of
drill holes increases"
Have a good day.
-----Original Message-----
From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx]On Behalf Of J Wages
Sent: Friday, January 05, 2007 5:37 PM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: 0402 round pads
Jelena,
I agree. I love using micro vias, but it's hard to convince some folks
of the real value. Signal integrity plus high yield. What they see first in the
initial fabrication costs. Tis a shame.
Jim S. Wages / SR. PCB Layout Designer:
Cary, NC - H: 919-466-1596 Cell: 919-484-2963
-----Original Message-----
From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Jelena Larsen
Sent: Friday, January 05, 2007 8:16 PM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] Re: 0402 round pads
Ah....the luxury of a micro via. If you get a chance look at an XBOX360
motherboard, bottom side under the CPU. An array of 0402 bypass caps side by
side tied to the plane with a standard via 10mil finished drill size. No
tombstone issues. Manufacturing tested. Patented design. Most impressive for a
4 layer board. Oh....the 0402 pads are rectangle. You can find pictures of it
on the internet.
Jelena
________________________________
From: icu-pcb-forum-bounce@xxxxxxxxxxxxx
[mailto:icu-pcb-forum-bounce@xxxxxxxxxxxxx] On Behalf Of Unruh Barry
Sent: Friday, January 05, 2007 4:24 PM
To: icu-pcb-forum@xxxxxxxxxxxxx
Subject: [PCB_FORUM] 0402 round pads
Gary
I feel that the significance of this discussion has been missed.
The fact that you can imbed termination resistors and decoup caps into
a 1mm BGA via grid on the back side is a very BIG DEAL!
The round pads enable you to do this. Maybe some other shape works
also, but not square or rectangle.
For every 2 vias you can fit one 0402 component.
No vias need to be removed.
Short is better whether your talking about caps or termination
resistors.
This technique may delay or reduce the need of moving to 0201 packages.
Build your 0402 alt symbol with 1 mm pad to pad spacing.
What we use is....
Pad size is .022".
Via size is .019".
Via to pad is .007 min.
Make the solder mask cover most of the via.
Of course I can't guarantee yield, but so far so good.
It would make placement easier to be using a metric database but not
vital.
If your on an inch database use the rat going to the pad to enable you
to place the part to the closest .0001 inch.
Barry Unruh
Other related posts:
