Re: [SI-LIST] : RE: Power planes

About this list Date view Thread view Subject view Author view

From: Alan Hilton-Nickel (ahilton@transmeta.com)
Date: Fri May 04 2001 - 09:28:32 PDT


Hi Doug,

Your signals are "fast enough". :-)

I'm not sure you need to reserve an entire plane for power just because
it is high current. You may want to check Douglas Brooks website for
information on current capacity and review your requirement. The
topology you would need to split this plane would be the determining
factor. If the "high current" you are concerned about is mostly DC, you
could also increase the thickness of those layers. This would do next to
nothing if your currents are all high frequency, as skin effect will
keep them close to the surface of the plane.

I'm also not sure I understand the point about "isolating" routing
layers. I think he means "pairing" or grouping them. Here's what I try
to get our board designers and customers to do.

First, try and view the routing layers in pairs. Between each pair sits
a ground plane. In general, you want to restrict the routing of a signal
to one routing pair, to maintain continuity of the return current. If
you find you have to switch a trace to another routing pair, either move
the entire trace to the new pair, or place a ground via very close to
the transition via. That way the return path is controlled.

You then stack the board in triplets (ground planes plus routing pairs)
and pairs (power and ground planes).

I see you have your outer layers set up with little routing. I assume
you are doing this to minimize manufacturing variations in trace width
due to plating, or you want to only deal with one trace velocity. Good
reasons, although I don't worry that much about it at these speeds.

If you want to keep those outer layers for breakout only, then I would
suggest this stackup:

1. ---- ---- Top layer (Very little routing) (2 oz)

2. ---- ---- Routing (1 oz)
3. --------- Split Power (1 oz)
4. --------- Ground (1 oz)

5. ---- ---- Routing (0.5 oz)
6. --------- Ground (0.5 oz)
7. ---- ---- Routing (0.5 oz)

8. --------- Power - 3.3v (0.5 oz)
9. --------- Ground (0.5 oz)

10. --------- Power - 2.5v (0.5 oz)
11. --------- Ground (0.5 oz)

12. ---- ---- Routing (0.5 oz)
13. --------- Ground (0.5 oz)
14. ---- ---- Routing (0.5 oz)

15. ---- ---- Routing (0.5 oz)
16. --------- Ground (1 oz)
17. ---- ---- Routing (0.5 oz)

18. ---- ---- Bottom layer (Very little routing) (2 oz)

As you can see, this works out to 18 layers, so you may want to
reconsider using the external layers as breakout only. I have also left
out a power plane (misc. voltages). However, you now have 8 routing
layers instead of 6, so you could replace one of those routing layers
with the missing power plane, or you could try and split the misc
voltages onto the 3.3V or 2.5V layers. Otherwise you will need two more
layers for a total of 20 (yikes!).

Hope this helps.

Alan Hilton-Nickel
Transmeta Corp.
 
Doug Hopperstad wrote:
>
> Alan,
> 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
> power/grounds:
>
> 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
> issue.
>
> Doug Hopperstad
>
> -----Original Message-----
> From: Alan Hilton-Nickel [mailto:ahilton@transmeta.com]
> Sent: Wednesday, May 02, 2001 9:16 PM
> To: Doug Hopperstad
> Cc: si-list@silab.eng.sun.com
> Subject: Re: [SI-LIST] : RE: Power planes
>
> Hi Doug,
>
> 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... :-)
>
> Alan Hilton-Nickel
> Transmeta Corp.
>
> Doug Hopperstad wrote:
> >
> > I am currently looking at the following stackup for a design and would
> like
> > 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
> be
> > 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
> > 5v.
> >
> > 1. Is there any concerns with making the outer layers 1 or 2 ounce
> compared
> > 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
> power
> > planes?
> >
> > 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
> > majordomo@silab.eng.sun.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
> > ****

**** To unsubscribe from si-list or si-list-digest: send e-mail to
majordomo@silab.eng.sun.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
****


About this list Date view Thread view Subject view Author view

This archive was generated by hypermail 2b29 : Thu Jun 21 2001 - 10:11:50 PDT