[SI-LIST] Re: Need advice on basic 6-layer stackup
- From: "Graham Davies" <GrahamDavies@xxxxxxxx>
- To: "steve weir" <weirsi@xxxxxxxxxx>, <si-list@xxxxxxxxxxxxx>
- Date: Sun, 24 Apr 2005 10:37:27 -0400
Steve,
Thank you very much for your helpful reply to my posting.
OK, you're right, I could be jumping to conclusions that the first board's
problems are cross talk. You agree it's a bad stackup, so I'm not sure that
getting to the bottom of this is going to help me.
Thanks for confirming that the second stackup is better. My question,
really, is doesn't this go a bit too far with such a small separation of
signal and plane layers? For the low-tech parts on this board, shouldn't I
be able to back off a bit and make the traces higher impedance and easier to
drive?
By Cu imbalance, do you mean having two planes close to one side of the
board and only one plane close to the other? This seems difficult to solve
and still retain three routing layers and two power planes (three with the
duplicate ground planes) in six layers. The boards I have don't show any
warpage.
When you say "improve the power delivery by swapping layers 3 and 4", that
would be this change:
1 component side signals
2 ground plane
3 inner signals ---> power plane
4 power plane ---> inner signals
5 ground plane
6 bottom side signals
I think I understand this; the vias up from the power plane to the
components would be shorter. But, when a trace from the top side (where
they all hit the component pads after all) switches to another routing
layer, it would inevitably be a layer referenced to a different return
plane. This would make it more difficult to provide continuity of the
return path under the trace so keeping things as they are has merit too.
Regarding the trace impedance, I guess I have three problems. For a 6 mil
trace 3.2 mil above a plane I get a lower figure. Then, why 50 ohms? Is
this a magic number. Finally, for this low-tech board, so I really need to
get into controlled impedance?
Using http://www.emclab.umr.edu/pcbtlc/ as the trace impedance calculator,
selecting Microstrip and specifying a relative permittivity of 4.2, height
of 3.2 mils, width of 8 mils and thickness of 1 oz, I get 41.69 ohms.
Graham.
----- Original Message -----
From: "steve weir" <weirsi@xxxxxxxxxx>
To: <GrahamDavies@xxxxxxxx>; <si-list@xxxxxxxxxxxxx>
Sent: Saturday, April 16, 2005 11:50 AM
Subject: Re: [SI-LIST] Need advice on basic 6-layer stackup
> Graham, as to intermittent failures, the first board is a pretty bad
> stack-up. But you could be suffering from surge power starvation, SSO
> problems, signal ringing, and / or cross talk. If you want to engineer a
> reliable product, then you have some homework to do to insure that the
> signal timing and quality is adequate, as well as the power delivery. The
> second stack up is a big step in the right direction.
>
> I would be a bit concerned about warpage due to Cu imbalance.
>
> It is likely unnecessary, but you can improve the power delivery by
> swapping layers 3 and 4.
>
> The second stack-up gets you pretty close to 50 ohms by my calculator on
> all the signal layers. Specify to your fab that 50 ohms is what you want
> and let them adjust the line width to tweak it in. Make sure that your
> power delivery and clock distribution are clean, terminate your signals
> properly, verify your static timing and such a low speed system should
work
> fine.
>
> Steve.
>
>
> At 07:37 AM 4/16/2005 -0700, Graham Davies wrote:
> >
> >
> >
> >I have joined a small company that has no established experience in
> >signal integrity. I have inherited a product that has a lot of
> >problems that I believe are due to lousy signal integrity. I am
> >looking for guidance in selecting a good basic stackup for a redesign
> >of the PCB. I have spent a lot of time Googling for this and ended up
> >here.
> >
> >The current PCB is 6 layer as follows: component side signals, ground
> >plane, inner signals, power plane, ground plane, bottom side signals.
> >Minimum trace width and spacing are both 0.006 in. Material is 1/16
> >inch FR4 with 1 oz finished copper thickness for all layers. Maximum
> >signal frequency is, I think, 40 MHz and there's really nothing very
> >special going on anywhere. It's all pretty low tech and the design is
> >five years old.
> >
> >I have two revisions of the board. Both have the basic layer order as
> >above but completely different layer separations. I think the layer
> >order is fine, but I'm not really happy with either set of separations
> >so this is where I'm asking for help.
> >
> >The first revision has 0.008 in. between the outer signal layers and
> >the ground planes. Inside this is a 0.0145 in. separation. Then the
> >inner signal layer is referenced to the power plane and has a 0.007 in.
> >spacing from it. The type of problem this board has is that it will
> >run for a while and then crash. I think there is serious crosstalk as
> >traces are closer to their neighbors on the same layer than to their
> >reference planes. Also, the power plane has no really close ground
> >plane to form a distributed decoupling capacitor.
> >
> >The second revision has 0.0032 in. between the outer signal layers and
> >the ground planes. Inside this is a 0.004 in. separation. The inner
> >signal layer is therefore referenced to a ground plane. The power
> >plane is not used as a reference and is very close to the other ground
> >plane. The board thickness is made up with 0.038 in. in the middle. I
> >have found only one problem with this board so far which is consistent
> >though temperature dependent and can be fixed with a series resistor at
> >the driving point of a badly routed clock trace. It slows the edge so
> >as to increase the overlap of the outgoing and reflected signal edges.
> >
> >So, anyway, the second board with 3.2 : 4 : 38 : 4 : 3.2 mil
> >separations is clearly the better of the two, but for such a low tech
> >board the trace impedance seems rather low (40 ohms?). If I go with
> >this I think I'll need to add high-strength drivers all over. I'm
> >wondering if something like 5 : 7 : 28 : 7 : 5 wouldn't be a better
> >choice with an impedance of around 58 ohms? Or 4 : 6 : 32 : 6 : 4 for
> >around 50 ohms? Can someone help me out here? I can't figure out how
> >my choice of separations affects the manufacturability of the PCB
> >either. Google has never before let me down so badly.
> >
> >Graham.
> >
> >
> >
> >------------------------------------------------------------------
> >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 FAQ wiki page is located at:
> > http://si-list.org/wiki/wiki.pl?Si-List_FAQ
> >
> >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 FAQ wiki page is located at:
http://si-list.org/wiki/wiki.pl?Si-List_FAQ
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:
