[SI-LIST] Re: 24-layer PCB Stack-up
- From: "Jackson, T L" <t.l.jackson@xxxxxxxx>
- To: ched_chang@xxxxxxxxxxx, si-list@xxxxxxxxxxxxx
- Date: Fri, 12 Mar 2004 09:09:30 -0800
Chai,
For the 8 signal layers that you mention, I would suggest a 22-layer
stack-up like:
1. Signal 1
2. Ground
3. Power
4. Signal 2
5. Ground
6. Power
7. Signal 3
8. Ground
9. Power
10. Signal 4
11. Ground
------------------- < Insert one more Power and Ground layer pair, if
necessary, to get to 24 layers
12. Power
13. Signal 5
14. Ground
15. Power
16. Signal 6
17. Ground
18. Power
19. Signal 7
20. Ground
21. Power
22. Signal 8
This stack-up has 8 signal layers, 7 ground layers, and 7 power layers.
This stack-up will produce the greatest amount of board capacitance,
reducing the need for discrete decoupling capacitors. The inner signal
layers are almost completely shielded, so as many traces as possible
should be run on them, leaving a minimum amount of traces on the two
outer signal layers. If you felt that you really needed to maximize the
shielding, why not run a ground trace around the perimeter of the inner
signal layers to reduce emissions or reception from the edges of the
board?
Unless this board is extremely large, I don't think 166 MHz will be a
problem with careful layout. Tricks like putting vias on the sides of
passive component pads, rather than outside of the pads, will do more to
reduce parasitic inductance from decoupling than trying to minimize the
connection lengths in the vias.
That's the way I would do it based on the information you've given.
TJ
Thomas L. Jackson, P.E.
Senior Staff System Engineer
Department 72FS, Mechanism Products System Engineering
Lockheed Martin Space Systems Company
Building 149
1111 Lockheed Martin Way
P.O. Box 3504
Sunnyvale, CA 94089-3504
Telephone: (408) 742-2013
Facsimile: (408) 742-7701
-----Original Message-----
From: si-list-bounce@xxxxxxxxxxxxx [mailto:si-list-bounce@xxxxxxxxxxxxx]
On Behalf Of Ched-Chang Chai
Sent: Friday, March 12, 2004 1:32 AM
To: si-list@xxxxxxxxxxxxx
Subject: [SI-LIST] 24-layer PCB Stack-up
Dear all,
I have a question about a PCB stack-up. Due to certain reasons, I must
design a 24-layer and 5mm thick board although we will be only using 8
signal layers. The other 16 layers will be Power or Ground. The signals
are
operating at 166MHz. I have a few concerns about this board:
(1) the inductance and capacitance of through-hole via (they are 5mm
long!).
(2) the effect of vias to power-ground decoupling (bypass, decoupling
capacitors).
(3) Electromagnetic Interference.
To minimize the above effects, I am thinking to set the stack-up as:
1. Signal
2. GND
3. Power
4. Gnd
5. Signal
6. Gnd
7. Signal
8. Gnd
9. Signal
10. Gnd
11. Signal
12. Gnd
13. Signal
14. Gnd
15. Gnd
16. Gnd
.
.
.
Gnd until 24 layers.
I set ground and power planes at layers 2 and 3 respectively to minimize
the
via length associated with the bypass/decoupling capacitors. The other 5
signal layers are set closest to Layer1 to minimize the via length when
traces change layers. I sandwich the signal layer between Gnd planes to
reduce EMI effect.
Is this a good choice? How to set a stack-up that can minimize the above
mentioned effects?
Please advise me since I am green horn in PCB stack-up.
Thank you very much in advance.
--
Regards,
Chai
_________________________________________________________________
Using a handphone prepaid card? Reload your credit online!
http://www.msn.com.my/reloadredir/default.asp
------------------------------------------------------------------
To unsubscribe from si-list:
si-list-request@xxxxxxxxxxxxx with 'unsubscribe' in the Subject field
or to administer your membership from a web page, go to:
//www.freelists.org/webpage/si-list
For help:
si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field
List technical documents are available at:
http://www.si-list.org
List archives are viewable at:
//www.freelists.org/archives/si-list
or at our remote archives:
http://groups.yahoo.com/group/si-list/messages
Old (prior to June 6, 2001) list archives are viewable at:
http://www.qsl.net/wb6tpu
------------------------------------------------------------------
To unsubscribe from si-list:
si-list-request@xxxxxxxxxxxxx with 'unsubscribe' in the Subject field
or to administer your membership from a web page, go to:
//www.freelists.org/webpage/si-list
For help:
si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field
List technical documents are available at:
http://www.si-list.org
List archives are viewable at:
//www.freelists.org/archives/si-list
or at our remote archives:
http://groups.yahoo.com/group/si-list/messages
Old (prior to June 6, 2001) list archives are viewable at:
http://www.qsl.net/wb6tpu
Other related posts:
