From: Doug Hopperstad (firstname.lastname@example.org)
Date: Thu May 03 2001 - 07:46:57 PDT
Thanks for your comments with regard to this issue.
My original stackup was a 14-layer that did have the power/grounds adjacent
to each other (as in the 16-layer stackup). The two additional layers are
needed to provide the added voltage requirements. I understand your comments
regarding keeping the power planes adjacent to the grounds. To answer a few
questions you listed in your email:
1. I am using 3 - 4 mils between the power/grounds. Ideally I want them
as small as manufacturing will allow.
2. The grounds on each side of the split power plane are not required.
However, there are two solid power planes in the design (for current
capacity) and the additional power planes are not high current and can be
put on one plane. Hence the extra plane. I decided to use the additional
plane as a ground and place the split between the two grounds to
isolate it as much as possible.
3. The edge rates on the board are varying. However there are some edge
rates that are in the 100pS range. I realize that this is not ultra fast.
This is not what some will call "Fast".
In my original stackup, I was indicating the use of grounds to separate the
routing layers, per Dr. Johnsons comments in his book regarding high-speed
layer configurations (Chapter 5.8). In the book, it mentions to keep
power/grounds adjacent and use ground planes, not power planes, to isolate
routing layers. I was unable to keep both rules in place with this stackup.
The power planes that are adjacent to the grounds are the ones that supply
the voltage for the high-speed components. The other power plane is not used
to supply the high-speed and such is not placed adjacent to a ground. This
might be the wrong approach, but I feel it is more beneficial to keep the
routing layers referenced to grounds and not power planes. I look to this
group for feedback on this issue.
4. With regard to the 8 routing layers, I am not sure how the stackup could
changed to provide the necessary design requirements. Do you have a
different stackup that would provide additional routing layers and still
utilize the needed grounds and power planes?
Here is one stackup I was considering, for reference, I assume this is what
you were referring is the more desirable option with regard to
1. ---- ---- Top layer (Very little routing) (2 oz)
2. --------- Split Power (1 oz)
3. --------- Ground (1 oz)
4. ---- ---- Routing (0.5 oz)
6. ---- ---- Routing (0.5 oz)
7. --------- Ground (0.5 oz)
8. --------- Power - 3.3v (0.5 oz)
8. ---- ---- Routing (0.5 oz)
9. ---- ---- Routing (0.5 oz)
10. --------- Ground (0.5 oz)
11. --------- Power - 2.5v (0.5 oz)
12. ---- ---- Routing (0.5 oz)
13. ---- ---- Routing (0.5 oz)
14. --------- Ground (0.5 oz)
15. --------- Power - misc. voltage (1 oz)
16. ---- ---- Bottom layer (Very little routing) (2 oz)
What is the feeling regarding this version? The dielectric thickness between
the outer layer and the first internal is only 4 mils. Is this an issue?
Thanks for the great feedback and I look forward to more discussions on this
From: Alan Hilton-Nickel [mailto:email@example.com]
Sent: Wednesday, May 02, 2001 9:16 PM
To: Doug Hopperstad
Subject: Re: [SI-LIST] : RE: Power planes
I have a couple of comments and some questions, the answers to which
will probably generate some more comments.
I would always place a ground plane next to a power plane. High
frequency transients exist in the power distribution network, not just
the signal lines. You need a low-impedance path from your power supply.
So layer 15 needs an associated ground plane. the two grounds on either
side of power layer 3 are overkill.
If, as Matt suggests, you use a 3-4 mil separation between the power and
ground pair, then splits will not bother you too much as the interplane
capacitance will provide a low-inductance path for return signals. You
could combine the 3.3V and 2.5V power on a split plane as well,
depending on how the placement segragates the power pins.
You don't mention much about the use of the boards and planes. I'd like
to know what your edge rates (and clock frequencies) are. Are all layers
meant to be high-speed layers? Are the outer layers meant only to
breakout signals from BGAs and pads, for immediate routing to the
high-speed layers, or are they also for high-speed routing? Are you
doing any differential signals?
8 routing layers out of 16 seems like an inefficient stackup to me, but
the purpose of the board will determine what is really necessary... :-)
Doug Hopperstad wrote:
> I am currently looking at the following stackup for a design and would
> some feedback:
> 1. ---- ---- Top layer (Very little routing) (2 oz)
> 2. --------- Ground (1 oz)
> 3. --------- Split Power (1 oz)
> 4. --------- Ground (0.5 oz)
> 5. ---- ---- Routing (0.5 oz)
> 6. ---- ---- Routing (0.5 oz)
> 7. --------- Ground (0.5 oz)
> 8. ---- ---- Routing (0.5 oz)
> 9. ---- ---- Routing (0.5 oz)
> 10. --------- Ground (0.5 oz)
> 11. ---- ---- Routing (0.5 oz)
> 12. ---- ---- Routing (0.5 oz)
> 13. --------- Ground (0.5 oz)
> 14. --------- Power - 3.3v (1 oz)
> 15. --------- Power - 2.5v (1 oz)
> 16. ---- ---- Bottom layer (Very little routing) (2 oz)
> The dual-striplines are separated by grounds and the power-to-grounds are
> adjacent to each other for high frequency noise coupling. The board will
> made from Getek with Er = 3.9 with a total thickness of 125 mils.
> Dielectric spacing between layers:
> 1:2, 15:16 = 14 mils
> 2:3, 14:15 = 6 mils
> 3:4, 4:5, 6:7, 9:10, 10:11, 12:13, 13:14 = 4 mils
> 5:6, 8:9, 11:12 = 12 mils
> Layers 14 and 15 are going to be dedicated power planes, each for a single
> voltage source (2.5v and 3.3v). The split plane will have 1.35v, 1.8v and
> 1. Is there any concerns with making the outer layers 1 or 2 ounce
> to the inner layers set at 0.5 ounce?
> 2. Put the split power plane between two grounds planes?
> 3. How much of a dielectric spacing would be best between two adjacent
> I am open to using layer 2 as a power plane instead of a ground. I look
> forward to any comments on this issue, thanks.
> Doug Hopperstad
> **** To unsubscribe from si-list or si-list-digest: send e-mail to
> firstname.lastname@example.org. In the BODY of message put: UNSUBSCRIBE
> si-list or UNSUBSCRIBE si-list-digest, for more help, put HELP.
> si-list archives are accessible at http://www.qsl.net/wb6tpu
**** To unsubscribe from si-list or si-list-digest: send e-mail to
email@example.com. In the BODY of message put: UNSUBSCRIBE
si-list or UNSUBSCRIBE si-list-digest, for more help, put HELP.
si-list archives are accessible at http://www.qsl.net/wb6tpu
This archive was generated by hypermail 2b29 : Thu Jun 21 2001 - 10:11:49 PDT